What Are The "TOP 10 DON'T DO'S" of SolidWorks
Jon Miller
drawing, mating, relating, user grouping, you get the idea.....
--
Posted via Mailgate.ORG Server - http://www.Mailgate.ORG
Bob Zee
news:9001e86664102a138c1...@mygate.mailgate.org...
> as compared to modeling, best practices, file management, sketching,
> drawing, mating, relating, user grouping, you get the idea.....
mating, relating...
bob z. likes the sound of that. maybe not so much the relating part.
mr. kellner put a post about 'what not to do' on here a couple times.
what are you looking for, mr. miller, things like "don't dimension to
center marks" and stuff like that?
bob z.
p.s. it was late in december, the sky turned to snow
all around the day was going down slow...
Jon Miller
Sporkman
>
> as compared to modeling, best practices, file management, sketching,
> drawing, mating, relating, user grouping, you get the idea.....
Like
1) Don't create Feature Patterns without checking the Geometry Pattern
box (unless you can't because of your design intent)
2) Don't create a Fillet as a Feature if you can do it via a Sketch
instead
3) Don't add identical components to an Assembly individually if you can
add them via a Component Pattern instead
Is that what you mean?
Jon Miller
Oh yeah..preach on brotha man, can i get an Amen!
Todd Best
onscreen message box. (assuming you get the message).
Is this what you mean?
"Jon Miller" <jmi...@ahaus.com> wrote in message
news:9001e86664102a138c1...@mygate.mailgate.org...
wgates666
"saving" and "printing."
HTH. HAND.
-john
In article <ucgtk8l...@corp.supernews.com>, todd...@rts-group.com
quipped:
Sporkman
>
> > Is that what you mean?
>
> Oh yeah..preach on brotha man, can i get an Amen!
OK, well I'd be interested to see if others 2nd the motion. I'm not
absolutely sure of the value of all of those -- it's rather subjective
with me -- and I'd like to know if others can back my points up with
personal experience.
Jon Miller
news:3CC872D1...@bigfoot.com...
> Jon Miller wrote:
> >
> > as compared to modeling, best practices, file management, sketching,
> > drawing, mating, relating, user grouping, you get the idea.....
>
> Like
> 1) Don't create Feature Patterns without checking the Geometry Pattern
> box (unless you can't because of your design intent)
I CHECK THE GEO BOX IF THE PATTERN DOESNT WORK WHEN I HIT O.K.
> 2) Don't create a Fillet as a Feature if you can do it via a Sketch
> instead
why not isn't that what the fillet command is for
> 3) Don't add identical components to an Assembly individually if you can
> add them via a Component Pattern instead
Always! And insert sketch driven feature that drive componet numbers
too!
>
> Is that what you mean?
As far as the validity of this post...I'm fishing for UserGroup meeting
topics. I thought i would see what all the opinions here would be, as
well as hitting up the other 16 eng's here.....why do i get the feeling
i've got a case of the black balls...thats blck bob not blue..ouch!
George
> 1) Don't create Feature Patterns without checking the Geometry Pattern
> box (unless you can't because of your design intent)
I avoid it unless really needed. In a perfect SW world I would
agree with you.
> 2) Don't create a Fillet as a Feature if you can do it via a Sketch
> instead
That depends on what it is you are sketching at the time. Just in general
I'd say most of the time on corners, sometimes on edges.
> 3) Don't add identical components to an Assembly individually if you can
> add them via a Component Pattern instead
YES! although I sometimes find myself wishing I could pattern a pattern,
but I guess that belongs in another discussion.
>
I'd like to add that people should take the time to give things names
that are meaningful rather than just "CirclePattern2" or "Cut-Extrude547".
Matt Smith
rep...cough... of my part without fillets and other useless stuff for fast
assembly manipulation.
-Matt S.
Jon Miller
> rep...cough... of my part without fillets and other useless stuff for fast
> assembly manipulation.
Would be very interested in success rate... I use many configs and to
multiply it by additional simplified and detailed configs would, i feel
, multiply the confusion...i could be wrong, i haven't tried it yet.
Eric Zuercher
create a separate file for each position, especially if equations are
involved. DO NOT use one file with multiple configurations --
Solidworks will screw up the equations and probably the hose path as
well. Multiple files works great and it's not really much more work.
Also, saving files lately seems to be a touchy issue. Try not to save
your work at all to avoid crashes.
Eric
"Jon Miller" <jmi...@ahaus.com> wrote in message
news:9001e86664102a138c1...@mygate.mailgate.org...
> as compared to modeling, best practices, file management, sketching,
Sporkman
> I CHECK THE GEO BOX IF THE PATTERN DOESNT WORK WHEN I HIT O.K.
I've been told by a couple of people that Geometry Pattern will resolve
quicker and more easily -- less computation time.
> > 2) Don't create a Fillet as a Feature if you can do it via a Sketch
> > instead
>
> why not isn't that what the fillet command is for
Certainly, but we're talking about time to resolve features here. When
you're dealing with one Part it usually doesn't matter much, but you go
multiply that by several tens or several hundreds in an Assembly then
you may notice it takes substantially longer to open.
Sporkman
in different positions? Use a configuration name (the same in all the
files you create) in the BOM instead of filename? (Well of COURSE,
Spork you blockhead.)
'Spork'
Jim Peyton
--
Jim Peyton
KINEMETRIX
Industrial Design and Manufacturing, Inc.
"wgates666" <jjablonski...@deluxestitcher.com> wrote in message
news:MPG.173233f25...@news.speakeasy.org...
Paul Salvador
..
Arlin Sandbulte
overall, I feel these are all "Best practice Ideas"
1.) Model using "smart" modeling practices. Basically, let SolidWorks do as
much of the design work for you as possible. For instance, use midpoint and
symetric relations instead of dimensions where possible. This just makes it
easier to capture design intent and easier for future updates. And I am not
just talking about top-down modeling. Here, we do very little top-down
modeling, but we still need to model parts "smartly."
2.) Always model parts/assys according to design intent. This is related to
#1, but goes a bit deeper. I just want you to THINK a while about how to
make a part before you just blindly jump in and model it up. Try to think
about the design intent.. what are the variables? How could the part
change? How is this part related to other parts? Initially, this process
may take some time up front, but it will reap rewards later.
3.) Use configurations for bolts and nuts and other common hardware and
drive the configs through design tables. This makes it MUCH easier to keep
you hardware model s consistant so that you can easily swap hardware
components in your assemblies. For instance, if you need a 3" long bolt
instead of a 2" long bolt, you can just change the config of your bolt part.
This essentially gaurantees that you will not have to remate the part as you
may have to do if you used seperate part files for each bolt. I personally
recommend making a one part file for all Hex head bolts, another for all
socket head bolts....
4.) CENTER YOUR PARTS ON THE MODEL ORIGIN!!! This is one practice I cannot
stress enough, especially on simple, prismatic parts. I am a firm believer
that your fist base extrude should be a mid-plane type extrusion and make
sure that your sketch is also centered on the origin. This simple practice
can VASTLY simplify mating practices as you can now esily mate to the cetner
planes of the part. Now, I realize that this is not possible for every part
and you may purposely elect not to center certain parts. My bolts for
example, heve the origin located at the bottom face of the bolt. BUT the
rest of the bolt is symetric! One of my pet pieves is when I see a simple
box that has been modeled by placing one corner coincident with the origin
with a blind type extrusion. This should NEVER happen in my opinion. If
you gain one thing from this discussion, let this be it....
5.) All parts/assemblies should be modeled using EXACT decimals. Tolerances
are later added to the drawing. Some persons where I currently work always
used 0.38 for 3/8" instead of 0.375. I cannot tell you how much of a
problem this has been for me.
6.) Do not lump all holes and features into one sketch. Use the SolidWorks
feature tree to help organize the design of your part. This will make it
easier in the future to make changes and understand someone else's model. I
hate it when I open a complex plate part with all holes and cuts sketched in
the base extrude.
7.) Name features to better show design intent and easier manipulation of
the model.
8.) Never use bolts and hardware to define the positions of parts in
assemblies. My rule is that you should be able to suppress all fateners in
an assembly and all of the piece parts should remain fully defined. This
simplifies your mating scheme and allows others to more easily decipher how
you build an assembly. Another benefit I like is that you can create a
simplified configuration with all of your fasteners and other non-essetial
parts suppressed to speed up SolidWorks performance when you dont need all
the extra detail.
9.) Use configurations to simplify large, complex parts and assemblies. As
I alluded to in item 8 above, it can be very beneficial to suppress
non-essential items when you don't really need all of the detail. This can
greatly impove SolidWorks performance.
10.) Use lots of subassemblies. My suggestion is try to split large
assemblies into lots of subassemblies and series of steps. This helps
improve SolidWorks performance (it does not have to solve all those mates at
the same time), and it makes the assemblies easier to manage. You don't
have as many parts or mates to search through. I try to set my models up as
though I was building it on an assembly line. I start with a basic frame
weldment then add a bunch of my mounts and tabs to it, then add the engine,
then add the suspension (as an example).
11.) Make extensive use of interference detection to both design errors and
modeling errors. Even on very large assemlies, interference detection does
not take long and it can easily dredge out errors you have made. I hate
interferences. According to the laws of physics, 2 masses of matter cannot
occupy the same space at the same time. Thus, I always try to modely my
parts according to the laws of physics and avoid interferences at all costs.
Plus, this practice fixes hidden line problems SolidWorks has in drawings
when parts interfere.
12.) Create and use part templates RELIGIOUSLY. I suggest setting up some
sort of review system in which part templates are created and checked by
others to review the model for things such I have discussed above. This
makes it much easier to swap out similar parts in your models.
13.) Create and use feature library features for common features. For
instance, I have created a large set of featrure library files for shaft and
hub keyways. Thus, each time I need a standard keyway, I can have it all
done in about 15 seconds with proper dimesions and tolerances already
defined.
14.) Never, ever have duplicate models of the same part in different
locations.
15.) Mate all nuts and washers to the bolt and not the hole. This just
simplifies and standardizes the mating scheme for your hardware. If I want
to change the hole my bolt is in, I only need to edit the concentric mate
between the bolt and the hole. Since the washers and nuts are mated
concentric with the bolt, they just move right along with the bolt and I
don't need to edit their mates at all.
16.) NEVER use "smart" part numbers. Part numbers are just a unique
identifier and should not contain any information. Part numbers that encode
information such as purchased, assembly, piece-part, weldment... are only an
invitation to disaster. After all, maybe you decide to manufacture a
previously purchased part, or something that was once an assembly can now be
made as a single part or vice versa. This leaves your part number
meaningless. It is better to start with meaningless part numbers. I
suggest using entirely numerical part numbers with no other characters other
than a single hyphen (see 17 below).
17.) SolidWorks files should be the same as the part number. Where
configurations are used to represent multiple parts in one file, the part
number should be the flie name appended with a dash and a sequential number.
18.) Organize your files in a central location and in a logical manner. I
suggest setting up 2 directories, Drawings and Models. These are
essentially mirror images of each other. I also suggest having one drawing
for each part number. Thus, you can have more files in the drawings
directory if you use configuration to define multiple part numbers per model
file. Under the drawings and models folders, subdivide the folder with
folders named 0,1000,2000,3000.....10000,11000.... Thus, part numbers from
0 to 999 will be placed in the 0 folder, parts 1000-1999 in the 1000 folder
and so forth. Thus, you only have 1000 files in any single folder and the
files are easy to find. Also (the real reason I suggest this setup) you can
easily make a macro progam that will open a specific part number file for
you. You never have to do any browsing to open a file!! Just make a macro
that lets you type in the part number and it will automatically open the
file for you. This is why I want the folder structure so organized. It
makes writing the macro much easier.
Well that ends my list so far. I probably have a lot more suggestions, but
these are the ones that come to mind immediately.
Just as a note, I work at a small manufacturing company (~130 employees)
where we design everything from single replacemnt parts to complete
off-highway machines. Drawings are how we comminicate with the shop floor.
Arlin Sandbulte
"wgates666" <jjablonski...@deluxestitcher.com> wrote in message
news:MPG.173233f25...@news.speakeasy.org...
Mike J. Wilson
Don't start a new drawing, part or assy until your template
is set up properly (name, custom properties, dim styles, units,
lighting, materials etc.)
Don't forget to study the "What's New" manual.
Don't draw a symmetrical part that isn't centered on the origin!
Don't forget to make a screenshot of your favorite toolbar settings.
Don't make helical threads just cause it "looks cool".
Don't forget to grab all the files you can...
http://www.mikejwilson.com/solidworks/solidworks_files.htm
Don't forget to try every feature in SolidWorks at least once.
Don't model an assembly as one part unless you are absolutely sure
you don't need to do a clearance/ interference check, show the
assembly in different configurations, or do any kind of animation.
Don't make all of your parts one boring color.
Don't make separate parts for fastener lengths and sizes.
Don't let everyone make their own fastener library, make one and
have everyone use that.
Don't "dumb dimension" a drawing, use existing associative
dimensions in the part.
Don't create a part until you have a proper file name or part number
for it.
Don't ignore the value of a PDM system.
Don't forget to document anything that could serve as a standard
for everyone to follow.
Don't put up with a slow computer or low RAM. Upgrade it!
Don't forget to create a DRM to train new employees on your
standards.
Don't forget to keep the DRM UPDATED!
Don't forget to go to those free seminars your VAR provides.
Don't create a million hole perf pattern.
Don't let anyone erase your configurations.
Don't open a part and yell "Who modeled this piece of crap!
doesn't this guy know how to use SolidWorks!!"
Don't blame SolidWorks for your own stupidity.
Mike Wilson
matt
I couldn't have written it better myself! I especially agree with:
- design for symmetry.
- configs for std hardware
- use part and feature libraries
- never keep models with duplicate names
- set up intelligent templates
- file name = part number
I would like to add a few of my own: (some of these assume multi user
environment)
- Edit rather than Delete.
- Feature palette and template files should be located on a read only
network drive
- if using PDM, don't put hardware in the vault
- never start SW by dbl clicking a file on a network drive
- don't work across the network if you can avoid it (except for read
only parts)
- the best way to work locally in a multi user environment is to use a
PDM system
- use driven dimensions to create your drawing
- use the fewest, simplest set of views possible to clearly convey your
point
- (opinion only) make all drawings B size - this can be readably reduced
to A for faxing and most places have the ability to print a B size.
- adjust your company practices where practical to allow the tool to
work for you - it is not a good idea to be so rigid in your practices
that you are always working against your tool, for example, last place
where I worked, the Mfg Eng Mgr required that all of the BOM type info
should be included in notes on the drawing. I presented a demo of how
this would work to his boss, along with a demo of how SW works
naturally, and it was decided to let the tool do the work for us rather
than to try to jam an inexpensive square peg into an expensive round
hole.
Thanks again, Arlin, and well done!
Matt.
Arlin Sandbulte
sort of suggestions....
Arlin
"matt" <mlom...@frontiernet.net> wrote in message
news:3CC8AF86...@frontiernet.net...
Krister L
sketch.....and I agree...the minus is that if You have it as a feature You
can supress it for faster performance in a "model layout"-configuration
Just my 2 cents
Krister
"Sporkman" <DOHsporkedUN...@bigfoot.com> skrev i meddelandet
news:3CC87987...@bigfoot.com...
JM Brun
> Don't forget to make a screenshot of your favorite toolbar settings.
--> Or Export the registry key:
[HKEY_CURRENT_USER\Software\SolidWorks\SolidWorks 2001\User Interface]
>
> Don't forget to create a DRM to train new employees on your
> standards.
What is a DRM?
ed
Great tips all.
"Jon Miller" <jmi...@ahaus.com> wrote in message
news:9001e86664102a138c1...@mygate.mailgate.org...
RJ
......not why am i clueless - I mean why is a sketch fillet better? Does
it make a smaller file size?
-RJ
"Sporkman" <DOHsporkedUN...@bigfoot.com> wrote in message
news:3CC872D1...@bigfoot.com...
Mike J. Wilson
> What is a DRM?
Drawing Requirements Manual
(or Drafting Room Manual)
Global documents makes a good general requirements manual
for starting things off. You can add company specific info to it.
Regards,
Mike
Matt Smith
feature.
If you draw a rectangle, extrude it, then add fillet features, you now have
2 features.
The kernel takes longer to regenerate 2 features than 1. Is it a big deal
in the aboce scenario? Probably not. But there are cases where the delay
will probably be quite noticable. As I stated before, I usually leave them
out as I always fillet last if possible.
-Matt S.
Matt Schroeder
Model items in the "Start with a block of metal the overall size or diameter
and length of your part and chip away the things I want gone" method.
Maddening...freaking maddening.
--Matt
Jon Miller
> and length of your part and chip away the things I want gone" method.
Curious...Could this be described as designing with detailing intent
that would then allow you to auto insert dimensions into the drawing
easier then working inside out and not having drawing friendly numbers?
I design the way you do (inside out) so I have not tested your "DON'T"
yet. Just curious.
wgates666
jmi...@ahaus.com quipped:
> > Model items in the "Start with a block of metal the overall size or diameter
> > and length of your part and chip away the things I want gone" method.
>
> Curious...Could this be described as designing with detailing intent
> that would then allow you to auto insert dimensions into the drawing
> easier then working inside out and not having drawing friendly numbers?
> I design the way you do (inside out) so I have not tested your "DON'T"
> yet. Just curious.
i must take issue with that method as well. that's more or less what i
do. the initial block is not always a square block, but my initial
sketch is definately setup more-or-less as a big block with everything
cut away. i import all my dims into the drawing from my model.
the main thing where i definately start with big block and cut things
away is with castings. config1=cast, config2=grind, config3=finished.
--john
Jerry Steiger
Matt,
Could you expand on your list? What do you mean and why do you do it this
way? In particular, what do you mean by "edit rather than delete"? Why do
you suggest using driven dimensions?
Jerry Steiger
At Work Computers
Matt Schroeder
dimensions.
All my designs have always had great auto dimension ability. I can't think
of the last time I used more than one or two driven dimensions.
I bet it's been years since I had more than 5 driven dimensions in any one
drawing.
--Matt
"Jon Miller" <jmi...@ahaus.com> wrote in message
news:ab4438d300b0a1bc370...@mygate.mailgate.org...
Eric Zuercher
> How do you handle the problem of a single part number for the same hose
> in different positions? Use a configuration name (the same in all the
> files you create) in the BOM instead of filename? (Well of COURSE,
> Spork you blockhead.)
>
> 'Spork'
We don't put BOMs on drawings, so I'm off the hook.
Eric
matt
The reason I like to "edit rather than delete" is that you will
typically do less work by editing because you'll have to redo fewer
features/mates. I'm talking about fixing screwed up parts, or making
major design intent direction changes.
With assemblies, one bad mate can make the whole tree bleed. Find the
bad mate and correct it rather than delete 10 mates that you'll have to
recreate.
Here's an example I saw today. Someone had made a nice model, but did a
bad job doing it (if that makes any sense). The problem was the base
feature. It would have been easy to tell them to just redo the whole
thing, but instead, I changed the original arcs to construction
geometry, and sketched a spline over the arcs, and only had to redefine
40% of the features using the existing sketches instead of having to
rebuild 100% of the sketches and features. Of course there is always a
limit where it is simply more economical to delete and recreate.
Ed Eaton recently wrote a post covering some of his
edit-to-avoid-rebuilding techniques. It was called "Delete Help". Lots
of nice ideas from Ed and others. Most of what I have to say has been
said in the same thread as Ed's post.
Here's my theory on using driven dimensions on the drawing:
- I rarely model the same way that I would detail a print. Good
modeling practices are not the same as good manufacturing practices.
Modeling using symmetry is very good practice, but detailing that way is
very bad practice. What if your drawing is an inspection drawing? You
have to detail according to how the part will be inspected. It would be
silly to model this way. Parametric/Associative modeling is done to
automate change. In my view, you cannot create a print using this idea.
- From a practical point of view, the best way to "Insert model items"
is to do it on a feature by feature basis, because bringing all of them
in at once is too much info. Once you do this, then you have to
rearrange them, and get the witness lines to go to the right places,
etc. By the time you're done, you've handled each dimension probably 4
times, and you might have to recreate some using driven dims anyway,
plus you've got to check that you've got all the dims you need, and
maybe pull some from another view. If you just use driven dims right
from the start, you handle each dim only once, and you can place them in
an organized way immediately.
- I consider it a best practice to make changes to the part from the
assembly so that it is readily apparent if your change makes sense. For
this reason, I don't usually want to make part changes from the drawing,
so the other advantage of inserting model items is lost on me.
Matt.
Dale Dunn
> i must take issue with that method as well. that's more or less what i
> do. the initial block is not always a square block, but my initial
> sketch is definately setup more-or-less as a big block with everything
> cut away. i import all my dims into the drawing from my model.
Any chance you can post a sample of this somewhere? I never did understand
what situation this would be advantageous for... I am of the school that
model dims and drawing dims are rarely the same.
EDWARD EATON
If the object starts off as a rod and gets cut down in reality, I'm going to
try real hard to do that in SW as well.
This process:
a) insures that what I am making can be done in the real world
b) automatically makes making my drawings meaningful to the guy making the
part.
I don't want to slam you - you have your own, very legitmate and
professionally sound reason for advocating what you advocate. I just feel I
gotta say that the opposite can also be legitimate.
Cheers-
Ed
"Matt Schroeder" <schr...@hotmail.com> wrote in message
news:3cc9...@news.mhogaming.com...
EDWARD EATON
when I went looking for it I couldn't find it. Sorry.
However, when digging through my archive of half finished musings about SW,
I ran across this document. Written maybe two years ago, it covers a lot of
the same territory as a top ten list, but in a far more insulting and less
sensitive manner.
So, what the hell. here it is.
I've even added a couple items that are fresh on my mind (and yes, I am a SW
goofus mare often than I would like to admit. But I am trying - with every
new model - to be
better)____________________________________________________
SW Goofus: When in a rolled back state, he deletes contour geometry in a
sketch and redraws the lines when he needs to edit a sketch's contour
SW Gallant: Is very careful to avoid deleting contour geometry when it is
possible. He knows that SolidWorks creates its internal names for faces and
edges based off the contour geometry that makes those features. If lines in
parent sketches are deleted and replaced with new lines (even if the new one
is in the exact same location as the original line!), all of the children of
that feature might experience rebuild errors because they are looking for
the faces or edges created by the original line, not this new one.
SW Goofus: Uses the 'all' field in display/delete relations when editing
relationships inside a sketch
SW Gallant: Uses 'criteria' when displaying/deleting relations so as not to
waste time on irrelevant relations. If he is fixing rebuild errors, he will
look under 'dangling' or 'external' (especially external!). If he is trying
to edit a sketch that has 'in context relations', he will limit his search
to 'in context'.
SW Goofus: Uses Fix relationships in sketches. He is a former ProE user and
insists on fully defining everything, even when he can divine no actual
intent for it.
SW Gallant: Uses fix rarely if ever at all. He knows that sketch
relationships are used to add intelligence to a sketch to accomplish some
goal. If something doesn't have to be tied down, it isn't. When it is useful
to have something fully defined, he uses dimensions so anyone editing the
sketch can quickly identify what's going on (gallant knows that, barring
2001+, fix relationships are very hard to root out in a sketch you are
unfamiliar with).
Gallant also knows that fix is never, never, never, never, enver used to
fully define a section for a sweep with guide curves. Never.
SW Goofus: Opens sketches to make changes in dimensions when modifying his
models
SW Gallant: Knows that once you close out of editing a sketch you can no
longer 'undo'.
So, when Gallant needs to modify dims, he double clicks the sketch (or its
feature!) in the feature tree and changes the values of the dims on the
screen. If the change has unsavory results, gallant gets to undo the change.
When editing under-defined sketch entities, Gallant turns on 'move-size'
features and drags the under-defined elements around. Not only do the
effects show up in (close to) real time, but he also gets to undo his
changes if they aren't good!
SW Goofus: Deletes features he thinks he no longer needs
SW Gallant: Suppresses features so he can always go back to them if their
absence causes a problem, or if the design changes back to where it was
before. He only deletes if the file has been backed up, has been fully
evaluated (and those features he wants to delete truly are never needed for
the job again), or if he needs to release it to someone unfamiliar with it
that might get confused by all of the suppressed features.
SW Goofus: Doesn't name any features
SW Gallant: Names features as he makes them so it will be quicker to find
features when he, or someone else, has to go in and edit the model. This
doesn't mean he names every single feature - but he labels enough of the
significant ones to save time later on.
SW Goofus: When assemblies get over-defined, goofus goes crazy deleting
mates or randomly changing their values to try to fix things
SW Gallant: Suppresses mates to diagnose which ones are causing the assembly
to be over-defined - usually the last one added. This way, he doesn't loose
any of his design intent or hard work. He also unfixes components to see if
that is the source of the over-definition, and uses either 'view mates' or
'view dependencies' to narrow his search
SW Goofus: Always starts his first feature on new parts on the FRONT plane
because that is the default
SW Gallant: Thinks through how he wants to model the part, and begins his
first feature on a plane that is smart for the part.
He tries to use a consistent frame of reference for all of his parts, so the
FRONT is always the front of the part, the RIGHT is always the side of the
part, and the TOP plane is always something smart - like the surface of the
part that sits on the floor. He does this so parts are all in the same
orientation when he drops them into assemblies, and so he can save time by
working in a consistent and intuitive frame of reference.
Another strategy that gallant employs is making his Front plane consistent
with the 'front' he will use in his drawing.
SW Goofus: Draws sketches on faces of his models, because faces are easy to
pick
SW Gallant: Tries very hard to put his sketches on planes (when it is
consistent with the design intent). Sometimes a sketch needs to be tied to a
face because of the design of the part - the feature needs to move with the
face, etc. But often times, SW goofuses start sketches on faces because they
are lazy or sloppy, and this causes huge problems later on when editing.
Faces are easy to lose (for instance, if a split line is applied, all
children of that face will go dangling), and even easier to mess up somehow
(add draft to a face and all bosses projected off of it will now shoot up
into the air)
SW Goofus: Usually mates faces
SW Gallant: (controversial) tries to use planes to mate his components in an
assembly, when consistent with design intent. Plane based mates are more
robust, and less likely to cause over-defining mate problems (ever mated a
couple faces together that have a slight draft, only to find that now
nothing else in the assembly can line up?)
However, Gallant remembers the caveat: 'when consistent with design intent'.
All mates are made for functional reasons, not for convenience. If a
functional mate can also be tied to a plane or an axis, that's great!
However, it has to be functional in the first place or it is a no-go.
SW Goofus: Mates edges and vertexes
SW Gallant: Is very hesitant about mating edges and vertexes, because if
someone edits the part to add a fillet, all of those mates will blow out. If
push comes to shove, gallant will try to use the sketches that create the
edge in the first place as a stable mate reference in lieu of the edge.
SW Goofus: When editing parts in an assembly, Goofus makes relations and
dimensions to the origin by picking the origin from the screen
SW Gallant - always, always, always makes relations or dimensions to the
origin by picking the origin icon from the feature tree. This absolutely
insures that the correct relationship is created. If they are close or
coincident, the assembly's origin (not the part origin) is the default when
picking from the screen, allowing an unintended and potentially disastrous
'in-context' relationship to sneak in.
SW Goofus: Is convinced that under-defined sketches spontaneously change
their shape and jump around
SW Gallant: Knows that, after he learned to check all of his sketches for
unintentional 'external' relationships, his sketches somehow, magically,
started to behave. He is no longer afraid of leaving sketches under-defined,
because they always remain exactly as he left them (unless he made a mistake
and there is some reason for them to move)
(don't get mad at me for this one, folks. its just - in my experience -
100%true. I have not had a single sketch do anything weird since I got a
clue. Not one sketch. Not one)
SW Goofus: Deletes dimensions, then remakes them
SW Gallant: Just modifies dimensions to make the leaders point to something
new, saving work on existing drawings that will now update correctly
SW Goofus: Makes modeling decisions for the sake of banging out the model
SW Gallant: Knows that his model is just part of a long, complicated
process. No one buys models - they buy product. If he models functionally,
thinking about streamlining drawings and manufacture, everyone working
together gets the product out to market (and making profits) faster than if
he were just to 'bang out the solid and screw the folks down stream'.
(controversial) Models should be made as they are made in the shop. if they
start out as a blank that then gets machined down, your model should start
out as a blank and cut away to get your final product. This will streamline
the entire process, and everyone gets to stay employed.
SW Goofus: Deletes over-defining dimensions
SW Gallant: Sees if the dim is truly intended, and, if so, RMB clicks the
properties of the dimension to turn it into a driven dimension so he retains
it's value. He knows he can always toggle back to driven if the dimension
needs to be reinstated, and any drawings will stay OK
SW Goofus: Saves his files in whatever directory he happens to be in at the
time
SW Gallant: Creates a new folder for each job he works on, and religiously
places all of his parts, assemblies, and decals in that folder only. When it
is time to archive the job or share it with someone else, he only has to
move that one folder to the server or CD, and everything goes with it.
SW Goofus: Uses lofts and sweeps for many of his features
SW Gallant: Analyzes what he is trying to make to see if the shape can be
achieved with analytical features (extrusions, revolves, fillets, etc).
Analytical features are more robust, faster to regenerate, more accurate,
and will have better results when merging bodies. You would be stunned with
how many 'complex' shapes can be modeled accurately with simple geometry
SW Goofus: Tries to use surface features whenever possible because they are
so powerful
SW Gallant: Tries to default to solid features whenever possible. Gallant
knows that he is not the only person who will touch this file, and surface
features are widely misunderstood by (and scary to!) a lot of other users.
Besides, you can't import dims from a surface features into a drawing (for
some god-awfully unfathomable reason.)
If surfaces are necessary, so be it. But if it can be done in solids, the
advantages are high.
SW Goofus: Uses 'Cut-Thicken:Offset surface' to have a surface trim material
away from a solid model
SW Gallant: Uses 'Cut with surface' to have a surface trim material away
form a solid. While Goofus is waiting for his parts to rebuild, Gallant has
already finished his job and is out with friends watching the game and
slamming back Leini's.
Thicken (the offset variety, not thicken a knit surface into a solid, which
is really a different thing altogether) is one of the most processor
intensive and unnecessary features in the entire package - to the point that
there should be a warning if you ever try to use it. Cut with surface is
way, way, ways better in 90% of cases.
SW Goofus: Tries to build parts directly off of the data his client gave him
SW Gallant: Analyzes the data to see what is happening between the date
points. Something that looks like it might have to be lofted might actually
be a simple revolved feature if you look closely enough to identify the
problem. Also, analyzing the data will catch internal conflicts and
inconsistencies - its surprising how wrong provided data can be!
SW Goofus: Uses fancy tricks whenever possible to show off his SW prowess
SW Gallant: Analyses every feature to see if there is a simpler way to
achieve the design intent. Gallant knows that it is unlikely that he is the
only person who will ever touch the files; the next guy might not be as
skilled or knowledgeable, and his company or client may lose time and
profits because the files are difficult to work with. Also, gallant is
experienced enough to know that exotic features are more buggy (simple
features get used more, and bugs are rooted out and fixed more quickly)
SW Goofus: At the end of the modeling job Goofus checks out his model to see
if it satisfies his design goals.
SW Gallant: Gallant rigorously checks out his models after adding every
important feature, to be sure that the model is doing what it is supposed to
do. This way, he does not put good work in after bad. While Goofus might
find a problem at the end of the day and have to work all night trying to
fix it, Gallant finds issues early, delivers his job on time, and gets to
spend his evening making sweet love to his lady (got Saturday Night Live
reruns on the brain).
SW Goofus: Does all sort of fancy and elaborate tricks to save himself some
time
SW Gallant: Does use fancy tricks to save himself time, but leaves notes in
the part (preferably by changing the text of a driven dim) so he and others
can quickly and intuitively identify the tricks. Things like linked values,
equations, and extra sketch lines used for mates or other relationships can
be very hard to identify when editing an unfamiliar part, and someone new to
the job might erroneously edit out important data if notes are not left to
the contrary.
Goofus: Tries to fix rebuild errors by starting at the bottom of the tree
and moving up
SW Gallant: Gallant recognizes, evaluates, and fixes rebuild errors from the
top of the tree down. Often, fixing an error at the top of the tree will
automatically fix all the errors below.
SW Goofus: When he sees rebuild errors, Goofus deletes features that are in
error, then tries to remake them.
SW Gallant: Knows that most rebuild errors are not a big deal, and that by
editing a feature (instead of deleting it) he can save all of the work and
children of that feature.
SW Goofus: Releases his assemblies for production when they are done
SW Gallant: Always, Always, Always runs interference detection on
everything, in every conceivable position, before releasing parts to be
made. Parts and tooling are expensive. A couple of hours of an engineers
tiome are cheap (and might save his job!)
SW Goofus' employer: Tries to save money by upgrading CAD stations only once
every year (or every other year).
SW Gallant's employer: Knows that good CAD stations are inexpensive compared
to labor costs. It doesn't take many hours lost waiting for a rebuild to pay
for a much faster machine - and good equipment makes it easier to retain
qualified (and expensive to recruit) design staff. The gallant employer
makes an effort to insure that his staff has the latest and greatest
equipment, so they can be better and faster than the competition. When times
are tight, he upgrades his power users first, then passes the 'next level'
systems down to the rest of the department.
The damn accountants can use the engineers hand-me-down systems. The gallant
employer never buys nice computers for accountants and sales staff unless
the engineers are on rocket ships.
SW Goofus' employer: Is very uptight about letting designers take company
software home
SW Gallant's employer: Is smart and knows that he can get his employee to
train on 'his own time' if he is only able to load the software in at home.
He negotiates with his VAR and makes sure that a home license is part of the
deal.
The truly 'gallant' employer is really smart and subsidizes computer
purchases for his staff. Personal note: my previous employer probably never
got a greater return on his investment than when he helped me buy a
computer, allowing me to learn SW (and push completion of jobs) at home on
my own time.
SW Goofus: When he runs into a problem, goofus spends a lot of time trying
to figure it out himself
SW Gallant: If he can't figure out a problem in five minutes, he sucks up
his pride and stands up to ask his coworkers if they know what's up with his
problem. If no one knows, he must take advantage of his support contract and
calls his VAR. They get paid if you call or not, so, dammit, use that
resource and make the most of your company's investment!
Mike J. Wilson
old military instructional Disney cartoons.
Mike Wilson
Edward T Eaton
was a kid. 'Highlights', I think it was.
I'm glad you liked it. I'm looking forward to the flames that will result
from this post - ought to be colorful:) Frankly, some of the items tick off
even me, though they are all 100% correct. Good modeling practices aren't
always the most emotionally satisfying, I'm sorry to say.
Have a good weekend-
Ed
"Mike J. Wilson" <mwi...@sigmathree.com> wrote in message
news:aafs7a$po6$1...@news.chatlink.com...
Pete J. Kavelish
"EDWARD EATON" <ed1701(no spam)@prodigy.net> wrote in message
news:lqHy8.1268$iR2.51...@newssvr17.news.prodigy.com...
I hate that! I was just asking my VAR yesterday...opps friday(we all know
they don't work weekends)...if he had heard anything regarding Solidworks
addressing this issue. It pisses me off when I do a load/replace of my
plastic part I get tons of rebuild errors. I have heard Pro-E handels this
issue by accepting that if a line is in the same place same length that its
the same line.
>
> SW Goofus: Uses the 'all' field in display/delete relations when editing
> relationships inside a sketch
>
> SW Gallant: Uses 'criteria' when displaying/deleting relations so as not
to
> waste time on irrelevant relations. If he is fixing rebuild errors, he
will
> look under 'dangling' or 'external' (especially external!). If he is
trying
> to edit a sketch that has 'in context relations', he will limit his search
> to 'in context'.
Oh yeah...I like that you can do that. I spent tons of time giving up on
solidworks until I found that filter (well and I went to class, but thats
what I learned there, so well worth the $500).
>
> SW Goofus: Uses Fix relationships in sketches. He is a former ProE user
and
> insists on fully defining everything, even when he can divine no actual
> intent for it.
>
> SW Gallant: Uses fix rarely if ever at all. He knows that sketch
> relationships are used to add intelligence to a sketch to accomplish some
> goal. If something doesn't have to be tied down, it isn't. When it is
useful
> to have something fully defined, he uses dimensions so anyone editing the
> sketch can quickly identify what's going on (gallant knows that, barring
> 2001+, fix relationships are very hard to root out in a sketch you are
> unfamiliar with).
>
> Gallant also knows that fix is never, never, never, never, enver used to
> fully define a section for a sweep with guide curves. Never.
>
> SW Goofus: Opens sketches to make changes in dimensions when modifying his
> models
>
> SW Gallant: Knows that once you close out of editing a sketch you can no
> longer 'undo'.
Wow great tip! I guess I have done it on accident. I mostly use the double
click method cause Im lazy. I have had other users ask when you can
accually "undo" cause it seems to not be an option when its needed most.
>
> So, when Gallant needs to modify dims, he double clicks the sketch (or its
> feature!) in the feature tree and changes the values of the dims on the
> screen. If the change has unsavory results, gallant gets to undo the
change.
Not to mention the time saved in rebuilds. This method allows you to change
alot of areas and then do one rebuild. Much better for me, cause it's one
long aZZ Break.
>
> When editing under-defined sketch entities, Gallant turns on 'move-size'
> features and drags the under-defined elements around. Not only do the
> effects show up in (close to) real time, but he also gets to undo his
> changes if they aren't good!
>
>
> SW Goofus: Deletes features he thinks he no longer needs
>
> SW Gallant: Suppresses features so he can always go back to them if their
> absence causes a problem, or if the design changes back to where it was
> before. He only deletes if the file has been backed up, has been fully
> evaluated (and those features he wants to delete truly are never needed
for
> the job again), or if he needs to release it to someone unfamiliar with it
> that might get confused by all of the suppressed features.
>
> SW Goofus: Doesn't name any features
That would be me! For my case I have started my own standard mold base and
have been giving relavent names. As for my cavity, no way, I'm just too
lazy for that.
>
> SW Gallant: Names features as he makes them so it will be quicker to find
> features when he, or someone else, has to go in and edit the model. This
> doesn't mean he names every single feature - but he labels enough of the
> significant ones to save time later on.
>
> SW Goofus: When assemblies get over-defined, goofus goes crazy deleting
> mates or randomly changing their values to try to fix things
>
> SW Gallant: Suppresses mates to diagnose which ones are causing the
assembly
> to be over-defined - usually the last one added. This way, he doesn't
loose
> any of his design intent or hard work. He also unfixes components to see
if
> that is the source of the over-definition, and uses either 'view mates' or
> 'view dependencies' to narrow his search
Another great Tip (view mates)! I use it alot. I don't like the interface
for it, but it saves lots of time.
Yep! lol
>
> However, Gallant remembers the caveat: 'when consistent with design
intent'.
> All mates are made for functional reasons, not for convenience. If a
> functional mate can also be tied to a plane or an axis, that's great!
> However, it has to be functional in the first place or it is a no-go.
>
> SW Goofus: Mates edges and vertexes
>
> SW Gallant: Is very hesitant about mating edges and vertexes, because if
> someone edits the part to add a fillet, all of those mates will blow out.
If
> push comes to shove, gallant will try to use the sketches that create the
> edge in the first place as a stable mate reference in lieu of the edge.
>
> SW Goofus: When editing parts in an assembly, Goofus makes relations and
> dimensions to the origin by picking the origin from the screen
>
> SW Gallant - always, always, always makes relations or dimensions to the
> origin by picking the origin icon from the feature tree. This absolutely
> insures that the correct relationship is created. If they are close or
> coincident, the assembly's origin (not the part origin) is the default
when
> picking from the screen, allowing an unintended and potentially disastrous
> 'in-context' relationship to sneak in.
Right just learning this. I have been using the transparent assembly, which
keeps me from haveing to do what I hate most of all, Thinking. For those
who don't know 2001+ has a setting that you can toggel on and off, which
allows you to force transparency to all objects exept the one your editing.
The only way you can select an object that is not your current editable part
is by selecting where you current part is not or holding the "shift" key.
What happens to the Gallents Toolbox files?
So are you saying we shouldn't delete?
Hell yeah...if nothing else its a great way to back up files!
Great post lots of wonderful Tips and Fun to read. (WHAT?)
wgates666
quipped:
> > SW Goofus: Deletes dimensions, then remakes them
> >
> > SW Gallant: Just modifies dimensions to make the leaders point to
> something
> > new, saving work on existing drawings that will now update correctly
not true.
grab a dimension in a sketch and drag one end to a new endpoint. the dim
is gone from the drawing. (unless this is fixed in SP2.0. i'm still
forced to use sp0.)
-john
wgates666
EATON" <ed1701(no spam)@prodigy.net> quipped:
> Sorry man - gotta disagree with you.
> If the object starts off as a rod and gets cut down in reality, I'm going to
> try real hard to do that in SW as well.
> This process:
> a) insures that what I am making can be done in the real world
> b) automatically makes making my drawings meaningful to the guy making the
> part.
i find this to be especially true on more complex pieces and on
castings.
--john
kwbosch...@earthlink.net
Ken B.
Matt Schroeder
I think some people have misunderstood my original beef with "outside in"
type models...
Here's a "for instance" for ya:
If parts are fine with steel stock dimensions or casting dimensions then I
also use the chip away method. For instance, if the base part is a block
with a hole and the stock size the shop has is fine, then I model it as such
and tolerance it accordingly. I also use this on castings and weldments and
any other time where convenient or proper to get design intent since that is
what matters.
I do use that method, but my beef with it was in more complex parts, and
even some people are using it on purchased parts!!... (All our screws are
made that way. Imagine the overhead in file size this has on an assembly)
Also, my main problem with some incorrect "outside in" practices is
dimensioning to features that are going to be removed in other processes.
This is not as likely to happen with inside out modeling, but some models I
have seen have poorly thought out design intent and the person modeled a
round part OD from the edge of the overall OD that was cut with a revolve
cut and therefore is not physically there anymore. (You can't manufacture
things like that so why model them like that?) There are times where you
can manufacture things like that BUT they limit the manufaturer to perform
processes in a certain order and I as a designer feel as though the final
outcome is all that matters. The machinist or mold maker or welder or
whatever can do anything they want to get my final part.
Here is an instance of that previously mentioned bad practice:
http://solidworksmodels.tripod.com/solidworksmodels/bad_practice.tif
Possibly you could show me an instance of how you can communicate more
effectively with the manufacturer with the "outside in" modeling practice.
I just might come over to your side of thinking.
--Matt
Matt Schroeder
#8 x 1/2 long socket head cap screw made with an overall base extrude, a cut
revolve to get the thread diameter, a cut extrude to get the hex key hole,
and a cosmetic thread, and a chamfer to get the head and thread lead in
chamfer (they used the same size for some unknown reason)
model file size: 227K
My version of the same: 1 base revolve, one cut extrude for the hex key
hole, and a cosmetic thread...
model file size 80K
Both were defragged etc....
--Matt
"Matt Schroeder" <schr...@hotmail.com> wrote in message
news:3ccd65ea$1...@news.mhogaming.com...
wgates666
quipped:
>
> http://solidworksmodels.tripod.com/solidworksmodels/bad_practice.tif
you think you jpeg that thing? i cant seem to open tif's here.
thx,
john
Evadem
added features like chamfers and fillets are much smaller than revolved
features. A plain cylinder without chamfers on my system is 43kb while a
revolved cylinder is 46kb. Add a chamfer and the extrusion is 169k while the
revolved jumps up to 196kb. So I always use extrusions if possible. A screw
done with revolved features is 230kb while done with extrusions is 142kb.
Dave
kwbosch...@earthlink.net
>
>"EDWARD EATON" <ed1701(no spam)@prodigy.net> wrote in message
>news:lqHy8.1268$iR2.51...@newssvr17.news.prodigy.com...
<BIG SNIP>
>
>What happens to the Gallents Toolbox files?
>
SWX Gallant used "File Find Reference" and did a "File Save As" to his working folder of all Toolbox or Pallet part
files.
Ken B.
Glen Weldon
"Matt Schroeder" <schr...@hotmail.com> wrote in message
news:3ccd65ea$1...@news.mhogaming.com...
wgates666
quipped:
> Here's an example:
>
> #8 x 1/2 long socket head cap screw made with an overall base extrude, a cut
> revolve to get the thread diameter, a cut extrude to get the hex key hole,
> and a cosmetic thread, and a chamfer to get the head and thread lead in
> chamfer (they used the same size for some unknown reason)
>
> model file size: 227K
>
> My version of the same: 1 base revolve, one cut extrude for the hex key
> hole, and a cosmetic thread...
>
> model file size 80K
>
> Both were defragged etc....
>
> --Matt
i'll do revolved parts like this too.
i think it depends on the model complexity if it's better to go with
block-and-cuts or just model-as-is.
--john
Pete J. Kavelish
to recreate the configs each time we put in a screw on a new project. The
problem with that is a lack of standard. I have a mold I'm currently
working on. I put in a screw with the toolbox add-in, that config does not
exist (because I copied the last toolbox screw file to a different directory
with the last job) so I fill out all the part # and description. Fine
working along and its all good. Then I get my boss standing over my
shoulder asking me to load up the old job and print out a new assy. Now I
don't close what I'm working on just load the other up. What screw file did
it use? We know what one, but the problem now is that the mold can't find
any configs it was using so now my BOM is screwed. Do you see what I'm
getting at. I'm not laying the blame on solidworks, I realize that it's our
lack of standards. What I have decided to do(done now) is go through my
toolbox screw files and add all standard screws in line with HoloKrome
standard. So from now on I will not have this problem. (I hope)
<kwbosch...@earthlink.net> wrote in message
news:g5tqcu832g5j4v72a...@4ax.com...
Matt Schroeder
wgates666
quipped:
oooh.
bandwidth limit exceeded. :)
--john
Paul Salvador
Paul Salvador
http://zxys.com/bad_practice.png (12K) PNG FORMAT ROCKS!!!
FYI, there is a new JPG addin you could use.
Now, to get a PNG addin. 8^)
..
Matt Schroeder
I keep forgetting about png...
I've been playing with GIMP for win32 and should have looked at the file
size.
The first one in tif was a jpeg compressed tif... hadn't realized it was
doing that and apparently nobody could read it... Makes nice files though.
But png is more proper.
--Matt
"Paul Salvador" <p.sal...@verizon.net> wrote in message
news:3CCD9BA0...@verizon.net...
wgates666
> Thanks Paul,
>
> I keep forgetting about png...
>
> I've been playing with GIMP for win32 and should have looked at the file
> size.
MMM..GIMP....
nice program.
--john
Glen Weldon
because I thought .JPG wasn't available! I knew there was a reason I lurked
around here!
Glen
"Paul Salvador" <p.sal...@verizon.net> wrote in message
news:3CCD9BA0...@verizon.net...
Paul Salvador
Yeah, with your image being just a few colors you can slim it down by
reducing the color count to 2 or 16.
PNG imo is one of the best all around formats for professional use, and
it's free public format.
The other small format is GIF but it Unisys I think still licenses it
and it's limited format.
Otherwise, if you post BMP, zipping them usually reduces the file
enough,.. maybe someday there will be a *.BMZ format for compression?
Never really used GIMP. Downloaded it and played with it and decided it
was not for me. I use PaintShopPro, very inexpensive, professional and
handles a wide range of formats.
..
kwbosch...@earthlink.net
I should have said save as "new filename". I always save the screw to a more generic filename like #10-32 X 1.25.SLDPRT
or something. It's not an elegant solution but it's working for us. I also have to add all of the custom property info
(via Excel table) for each fastener for our BOM. I'll have to go back and re-read what Mike's solution was. I'm always
open to new or better workarounds....
Ken B.
Matt Schroeder
are larger. Sometimes significantly.
I'm talking about limiting the number of features in a model when possible
because I guarantee you that any part that is created in 4 features but
could be created in two features is going to be larger than the part created
in two features.
I used screws as a good example because if you decide that your assemblies
need to be populated with screws then they can add unnecessary file size if
created in an unnecessarily sloppy manner.
--Matt
"Evadem" <san.rr.com@dmerrifield> wrote in message
news:7nez8.63147$VQ2.38...@twister.socal.rr.com...
Paul Salvador
Create a 1"x1" solid cylinder, save.
Create a A Size Drawing and drop the 1"x1" cylinder into it, save.
Saveas, TIF
Options:
-Black and White
-Compressed or Uncompressed
-Print Capture
-600 dpi
-A Landscape
-(no scale to fit)
-100%
-OK
You will get a error and or the SW meshing block shows it's working, try
to cancel....
Bye bye... cute!?
Evadem
extrusions and added features compared to revolved feature with chamfers in
the sketch. I don't add chamfers or cosmetic threads just to keep the file
size small.
Here is a great example of sloppy. I got a part with 8 holes in it and I
have to change the locations of the holes. So I double click the cut that
makes the holes and change the dimensions, regen, and save. I then go to the
drawing and when I check the dims for the holes, they didn't change. I
re-dimension the holes and they are still showing the original dimensions. I
then insert the dimensions from the part and up pop the changed dimensions,
but they are not going to the center of the holes. Bout this time I am
scratching my head trying to figure out just what the %$#@ is going on. I
open the part and edit the sketch and the person who made these holes had
created construction lines for the holes and dimensioned to the construction
lines, cept they forgot to create any relations from the circles to the
construction lines. So when I changed the dims I just moved the construction
lines and not the circles. All 8 circles each had their own dia dim too,
altho they were are the same size. Well I added relations and made the
circles all equal and all was good until I checked another part with a
series of holes in one sketch and these were done the same way. I was not
saying anything kind about this person by this time. I ended up having to
fix about 20 parts created this way. Too much fun.
Dave
Edward T Eaton
<clip>
> Also, my main problem with some incorrect "outside in" practices is
> dimensioning to features that are going to be removed in other processes.
Saw the image you posted, and I agree completely with you. Truly is
maddening.
And you agree with the 'chip away method' as follows:
> If parts are fine with steel stock dimensions or casting dimensions then I
> also use the chip away method. For instance, if the base part is a block
> with a hole and the stock size the shop has is fine, then I model it as
such
> and tolerance it accordingly. I also use this on castings and weldments
and
> any other time where convenient or proper to get design intent since that
is
> what matters.
So I think we are all saying the same thing, and are untied in the way we
curse SW Goofus.
BTW - I did some patternmaking and light machining through college working
for my old man. I didn't realize it then, but that work really helped me
'get' SolidWorks when I first started using it. I tend to approach SW
models like I approached jobs in the shop - first I think about what my end
thing needs to accomplish, then I think about how I can get there in the
most meaningful, stable way (with as little scrap and as few steps and
setups as possible), lay out before cutting anything, check my measurements
and progress as I go, etc.etc.etc.
That being said, I really can't think of a legitimate circumstance where I
would meaningfully dimension to the end of something only to cut away that
referenced end - so I don't do that in SW.
There are other odd modeling practices I've seen that I also instinctively
avoid because I know what it feels like to hold raw material in my hand and
try to make something of it in the real world.
The guy designing the part you showed must not do his own drawings - he'd
only have to do one or two before changing the way he thinks about modeling.
That's why drywallers sand their own tape jobs, and my old man got me into
painting and filling the things I machined. Nothing like a first hand
holistic understanding of the entire process to make you take responsibility
for your contribution.
"Matt Schroeder" <schr...@hotmail.com> wrote in message
news:3ccd65ea$1...@news.mhogaming.com...
Edward T Eaton
in
> error, then tries to remake them.
>
> SW Gallant: Knows that most rebuild errors are not a big deal, and that by
> editing a feature (instead of deleting it) he can save all of the work and
> children of that feature.
>So are you saying we shouldn't delete?
Nope. If the feature isn't needed any more it doesn't belong in the model.
But if the feature is in error because of a model change, and its a feature
you actully want, by all means try to edit first. Why spend 5 minutes
recreating something when you can fix it in half a minute, and save all the
children?
> SW Gallant: Creates a new folder for each job he works on, and religiously
> places all of his parts, assemblies, and decals in that folder only. When
it
> is time to archive the job or share it with someone else, he only has to
> move that one folder to the server or CD, and everything goes with it.
>What happens to the Gallents Toolbox files?
I don't have toolbox, so I'll hope the others who commented have settled the
issue
.
I used to work in a display design house where we would have shared files
(casters, TV monitors, shoes, etc) that we would drop into our assemblies.
Very convenient to have a library, and not dissimilar in principle from a
fastner library.
However, I learned to always make a local copy of the shared item and
archive that with my job. When my job is done and released for manufacture,
it needs to remain in a frozen state.
I have had projects go haywire because someone else opened the 'caster'
file, modified it for his job, and now it no longer fit in mine (or
incontext relationships cause my model to change size from what was released
to accomodate the new caster). SCREW THAT! I am never, never, never going
to put my jobs in a position of jeapordy again like that. Each and every
referenced file gets buttoned up in that job folder, period. Maybe I'm not
gallant, but I aint no goofus for it either.
Glen Weldon
I tried this exactly as you specified. The SW meshing block didn't show, I
wasn't given a choice to cancel. The process took about 5 seconds and
worked as expected. Wonder what could be going on there?
"Paul Salvador" <p.sal...@verizon.net> wrote in message
news:3CCDC9F3...@verizon.net...
Glen Weldon
at least for a few more days and have been doing without it for a couple of
years. I have built up quite a good parts library of standard components.
I use a separate folder for the job I am currently working on, but pull
standard components from a different directory. When I'm finished with the
job and it's time to archive on the server, I use the File>Find
References>Copy Files to the server folder that I created in advance. This
method copies the standard parts from the folder in which they reside and
creates a local copy on the server. Has worked very well for me and in the
days of inexpensive hard drives, disk space isn't an issue....
Glen
"Edward T Eaton" <ed'remove_this'17...@prodigy.net> wrote in message
news:4Wmz8.2447$Yb3.17...@newssvr16.news.prodigy.com...
Paul Salvador
It could be related to specific build and OS, mine is..
SW2001plus sp2.0
NTsp6a
Ok, I went through it again,.. change the following settings..
Uncompressed
Packbits
Here is the pop-up warning and the SW working solid/mesh animate block.
http://zxys.com/unable-to_and_processing-tiff.png
Let the pop-up warning box stay and let the SW solid/mesh working box
animate ~20 seconds and "cancel" and also hit the "ok" to close the
pop-up warning.
Now it should hang and/or possibly lead to a crash but I was able to
recover a few times, it's not consistent.
If it does not crash, switch between Uncompressed and Packbit.
Also, if you force close(through taskmanager) the hung SW session and
reopen another a new SW session, the first senario should hang and crash
but you may have to repeat the above. Something is now in the system or
memory which is currupt or memory is blocked. (I would suggest you
reboot your system after this because it may cause other problems)
Anyway, over the years when I have tried to Save As TIFF, it has in one
way or another crashed within the first few seconds of writing the file,
i.e., it has crashed on other releases.
Regardless, this is basic stuff SW Corp should be testing and the users
are being taken advantage of, and it's wroing.
..
jkskot...@gmail.com
> as compared to modeling, best practices, file management, sketching,
> drawing, mating, relating, user grouping, you get the idea.....
>
>
> --
> Posted via Mailgate.ORG Server - http://www.Mailgate.ORG
This can be debatable. Mostly radius can be created as sketch but not fillets. Fillet will mostly be the part of configuration change in any 3d model.