Calling all weldment experts
Keith Streich
My company manufactures material handling equipment (lifts which personal
can't ride). They cut, machine and weld up a bunch of structural steel,
paint it and assemble purchased components to create product. See
www.pflow.com for further information. There has been a push to implement
Solidwork's weldments package because the cut lists interface well with
DBWorks. After playing with the add-on for about 2 hours, I can't get it to
do what or how our shop fabricates weldments. I've known about a few
shortcoming, but I've found a few more since my little experiment. I could
be missing something since I've only have the 2004 training class on
weldments. Here are a few of my findings, please correct me if I'm
incorrect.
1. No gap can be created between joining pieces for shop fit up.
Structural steel is hot rolled from the mill and the tolerances on the OA
heights and flanges can be quite generous (5/32" height wise and ź" on the
widths). I typically cut back 1/16" on all steel butting against a flange
and let the fabricator fill the joint with weld (obtaining better
penetration also).
2. Many of the weldments are orientated to the top side, to support
the load; it must be flush with a plate on top for ease of loading with
pallet jacks and fork trucks. Since we optimize materials for strength vs.
weight, many times the internal members are smaller than the external
structural members. I cannot shift the internal profiles to match the top
side without multiple sketches on multiple planes or multiple profiles
offset at different heights.
3. Unlike structural steel parts created with sketches and features, I
can't suppress filleted edges in weldment profiles. I typical create
configuration with all fillets suppressed to speed up the assembled steel
parts or for quicker FEA analysis.
4. Internal member's sizes and lengths are dependent on other internal
and external member's sizes. So with weldments, I require multiple sketches
to have these members have relationships to other members. These extra
sketches must reside below the referenced members in the feature tree.
5. We don't cope steel as complex as Solidworks extends faces to
another member, we typically just notch a rectangular cutout in the corner
to match the flange and fillet in channels and beams. No custom copes in
weldments.
6. Parts can't have display states, only assemblies. multi-bodied
parts can hide bodies, but not with weldments. How can I show just one of
the structural parts which require machining? I was able to detail out the
part, but only after hiding the edges of all the other parts I didn't want
shown. With display states, I can create a separate state for each part
which requires machining. With multi-bodied parts, I can create separate
configurations for each part which requires machining. All weldments
require some type of machining or modification for stuff can attach to it or
it can attach to other stuff.
There might be other issues, but I've only played for a short time. Please
feel free to comment or ask questions. I hope to resolve these issues
before we jump on board without a paddle.
Keith Streich
Engineering Department
Pflow Industries, Inc.
John Layne
"Keith Streich" <ke...@pflow.com> wrote in message
news:4833344b$0$20197$4c36...@roadrunner.com...
Hi Keith,
Don't do a lot a weldments so can only help you with the first part of
number 6. Use "Relative View" to detail the members of the weldment in the
drawing and make sure the Scope has "Selected Bodies" checked.
The companies I know that manufacture a lot of weldments don't use the
SolidWorks Weldment feature, for the most of the reasons you state, they
model them as assemblies. Shame this part of SolidWorks software doesn't
seem to have been writen by someone who has much knowledge of welding.
John Layne
www.solidengineering.co.nz
Keith Streich
Keith
"John Layne" <JohnMINUS...@SolidEngineering.co.nz> wrote in message
news:jM-dnWwo_MxDCK7V...@supernews.com...
TOP
by the state line on the newsgroup.
> Pflow Industries, Inc.
TOP
Rod Morningwood
Keith,
1. You can try creating custom weldment profiles to suit your reqs. This
will affect your cut list lengths though. You'd have to sort out the pros
and cons for yourself.
2. Might want to try using separate sketches for each profile type.
(sketch1-4x4 only, sketch2-2x4 only, etc). see #4
3. SOL, the fillets are integral to the profile.
4. Personally, I put all my sketches at the top of the tree, then the
members, then the trims, then machining ops. Seems to work out well for
me. This method will require sketches to reference other sketches rather
than members.
5. Try breaking large weldments into smaller sub-weldments and bring them
together in an assembly. Sort of a best-of-both-worlds.
6. A detail view or separate sheet for said part would be my first
thought as well. Although convenient, I shy away from multi-part bodies
and mirrored assys, parts and features. Call me old-school but they
always seem to bite me in the ass down the road.
I've had issues trimming to bodies. I always trim to planar faces now.
I think you may want to play a bit more or try a prototype project before
jumping in with both feet. In my opinion, you're asking a lot of the
welding module, and in doing so, have already found some shortcomings and
work-arounds.
Perhaps you are the weldment expert ;)
rod
Keith Streich
at a lower cost. I thought that's we all should be doing.
Keith
PS It's not an elevator, it's a vertical conveyor (moves just things), or
else the elevator would red tag every unit sold.
"TOP" <kell...@cbd.net> wrote in message
news:302aba20-6ea5-4b1e...@r66g2000hsg.googlegroups.com...
Keith Streich
look like Swiss cheese, oh yeh, I forgot to turn on the oxygen!
I will try some of your suggestions, it just seems like more setup than
assemblies require, especially if all the members are variable in size and
position.
Keith
"Rod Morningwood" <p...@ph.uk> wrote in message
news:Xns9AA578319...@208.49.80.253...
Rod Morningwood
> I'm not the welding expert, just ask my superiors. Besides, my actual
> welds look like Swiss cheese, oh yeh, I forgot to turn on the oxygen!
>
> I will try some of your suggestions, it just seems like more setup
> than assemblies require, especially if all the members are variable in
> size and position.
>
> Keith
LOL, mine are pretty much a dog's breakfast.
Keith Streich
table pick the profile to use for given members? I want the user to punch
in "4" and the design table to propagate the appropriate pieces with a
C4x5.4# profile. I think there's a hard way to do this, by linking each
profile's dimensions to a design table column and having those cells update
via a master input spreadsheet. There would only be one configuration, but
the design table would drive all the variations of the weldment.
"Keith Streich" <ke...@pflow.com> wrote in message
news:4833344b$0$20197$4c36...@roadrunner.com...
Rod Morningwood
> Ok, I've got one more for the group. Is there an easy way to have a
> design table pick the profile to use for given members? I want the
> user to punch in "4" and the design table to propagate the appropriate
> pieces with a C4x5.4# profile. I think there's a hard way to do this,
> by linking each profile's dimensions to a design table column and
> having those cells update via a master input spreadsheet. There would
> only be one configuration, but the design table would drive all the
> variations of the weldment.
>
Keith
LOL - reminds me of a response given a few years ago when someone asked
if there's an easy way to design the hull of a ship.
"Click Insert\Boat" I believe was the quip.
It's been my experience that if you can arrive at the numbers you want in
the Excel sheet then the rest is easy. Just link the dims to the proper
cells.
I used to cost out my machines at my old employer using a fomula-laden
Excel BOM. I don't see why you couldn't utilize a design table in the
same fashion.
Your Excel-Fu must be good
Rod
TOP
on the way down unless you didn't get in under your own power. :)
Does the guy who pushes them out into the window use the stair?
BTW Isolate works on my box with weldment features or just
multibodies.
TOP
Keith Streich
bodies though, I just have to create a configuration for each piece which
requires machining.
Keith
"TOP" <kell...@cbd.net> wrote in message
news:4d55e586-882b-4816...@34g2000hsh.googlegroups.com...
Jerry Steiger
> Ok, I've got one more for the group. Is there an easy way to have a
> design table pick the profile to use for given members? I want the user
> to punch in "4" and the design table to propagate the appropriate pieces
> with a C4x5.4# profile. I think there's a hard way to do this, by linking
> each profile's dimensions to a design table column and having those cells
> update via a master input spreadsheet. There would only be one
> configuration, but the design table would drive all the variations of the
> weldment.
There is a fellow on the SW Forum, M. G. Martinez, who does some pretty
amazing top down design using Excel. A lot of his parts are sheet metal, but
I suspect you could learn a lot from some of the sample assemblies that he
has posted for downloading.
Jerry Steiger
John Layne
Hi Keith,
Please keep the group posted with your conclusions on the Weldment
functionality.
John Layne
www.solidengineering.co.nz
Keith Streich
1. A gap can be created by sketching non-conecting lines. A dimension
from end point to line can create the gap. Sort of FUBR to have any sketch
with non-meaningless dimensions all over to the overall intent of the sketch
or weldment.
2. No easy shift in profiles orgins to position members toward one side.
A 3D sketch could be creatred to offset the smaller members, but then again
you would have a sketch that was crazy looking unless one understood the
meaning of these offset lines.
3. Forget about turning fillets on and off. A profile is a profile, live
with extended time to display models and assembles, not to mention
regenerate drawing views. FEA packages love rounded stuff (so I'm told).
4. Relationships to other existing members. A design tables project from
heaven! Yep, can be done, but don't look at my equations.
5. Cope Solidworks way or cope Soildworks way! If your facility can't
afford a fancy waterjet, plasma or laser, what are you doing in business
anyway?
6. This one way solved, by your "Relative View" and "Selected Bodies"
suggestion. Works great! Display states would be a nice touch to weldments
though.
Cliff
wrote:
>FEA packages love rounded stuff (so I'm told).
Sharp areas can concentrate stress/strain & need
finer meshing.
--
Cliff
Willem1
Below my thoughts about your problems:
> 1. No gap can be created between joining pieces for shop fit
> up.
> Structural steel is hot rolled from the mill and the tolerances on
> the OA
> heights and flanges can be quite generous (5/32" height wise and ź"
> on the
> widths). I typically cut back 1/16" on all steel butting against a
> flange
> and let the fabricator fill the joint with weld (obtaining better
> penetration also).
You can draw your own structural member profiles (just edit an
existing profile sketch one and do a save as with another name). Make
the new profiles according to the maximal tolerances and the
connecting steel parts will always fit and not be to long.
>
> 2. Many of the weldments are orientated to the top side, to
> support
> the load; it must be flush with a plate on top for ease of loading
> with
> pallet jacks and fork trucks. Since we optimize materials for
> strength vs.
> weight, many times the internal members are smaller than the
> external
> structural members. I cannot shift the internal profiles to match
> the top
> side without multiple sketches on multiple planes or multiple
> profiles
> offset at different heights.
Make your 3D sketch lines at the top side and when placing the
weldments use "Locate Profile" to position one of the top corners of
the weldment equal to the sketch.
Another options is that you can make in the sketches of the structural
member profiles extra points (*). These points can be used to locate
the profile in the weldments.
>
> 3. Unlike structural steel parts created with sketches and
> features, I
> can't suppress filleted edges in weldment profiles. I typical
> create
> configuration with all fillets suppressed to speed up the assembled
> steel
> parts or for quicker FEA analysis.
Make your own structural member profiles without all the fillets (see
1.)
>
> 4. Internal member's sizes and lengths are dependent on other
> internal
> and external member's sizes. So with weldments, I require multiple
> sketches
> to have these members have relationships to other members. These
> extra
> sketches must reside below the referenced members in the feature
> tree.
In the 3D sketch you can make relations between the different
dimensions (see Equations).
>
> 5. We don't cope steel as complex as Solidworks extends faces
> to
> another member, we typically just notch a rectangular cutout in the
> corner
> to match the flange and fillet in channels and beams. No custom
> copes in
> weldments.
Do a Trim/Extend to the face of the body of the other member. Second
make a sketch with the required cutout and do a cut-extrude (through
all). Select the bodies for the cut-out and you have your own corner.
>
> 6. Parts can't have display states, only assemblies.
> multi-bodied
> parts can hide bodies, but not with weldments. How can I show just
> one of
> the structural parts which require machining? I was able to detail
> out the
> part, but only after hiding the edges of all the other parts I
> didn't want
> shown. With display states, I can create a separate state for each
> part
> which requires machining. With multi-bodied parts, I can create
> separate
> configurations for each part which requires machining. All
> weldments
> require some type of machining or modification for stuff can attach
> to it or
> it can attach to other stuff.
This one is already solved using the Relative view option.
Hope this helps a little bit.
Willem
Rod Morningwood
news:krL_j.66$2f5...@newsfe07.lga:
2. Create some additional points in the weldment profiles to locate from.
You could also use this to solve #1
/just a thought
TOP
Maybe I'm missing something because I have no problem using isolate in
any multi-body part with or without a weldment feature in SW2008 SP2.1
and higher.
TOP
Keith Streich
Keith
PS We have not jumped to SW2K8 for fear our ERP / DBWorks / DriveWorks will
not work together (even though the last two are gold partners and our ERP
will never be even a tin partner). Basically our ERP is an old UNIX system
migrated over to windows with ODBC capabilities and our to go guy has been
working on a linking API for two years and upper management steps very
carefully which surprises me their are devoted to weldments.
"TOP" <kell...@cbd.net> wrote in message
news:0a0a80ad-c562-4f64...@i76g2000hsf.googlegroups.com...
TOP
hiccups at first. I was running this 200+ body part through it.
I can't tell you about DriveWorks or your ERP although I would suspect
dbWorks handles the ERP side so if dbWorks is OK with it the ERP
should be too.
TOP