Built-in limitations in SolidWorks?
jp...@fast.net.au
an arc with 600m diameter. As I drew a circle with a smaller diameter,
dimensioned it and started to increase its diameter with the entry box,
from 500m (500.000 mm) upwards it snapped into an inwalid geometry
(yellow line). There was not any falty geometric comstraint in the
geometry which could have caused this behaviour.
So I ended up with a radius of 499.995mm - which is not right from the
tasks point of view.
To check this out I just tried to draw circles with different diameters
into the same sketch. For radii slightly bigger than 500m the circle
was drawn in bright yellow and I got the error message saying: Invalid
geometry. As I attempted drawing circles bigger than this, there was no
error message - but the circle did not draw at all. Lines longer than
500 m can be drawn, but they show up thin and are not usable. They can
not be highlighted, snapped to, measured etc. After changing the
display content (zooming in) the line simply disappears.
Is this one of the drawbacks of the relative low price of SolidWorks?
Janos Nemeth
J&P Design P/L
Sent via Deja.com http://www.deja.com/
Before you buy.
Edward T Eaton
I was told that there are some arbitrary cutoffs on what SolidWorks can
handle, dimensionally speaking. It's sort of like all of the old
programmers cutting the years down to two digits as a convenience, which is
causing all of this y2k bruhaha - in SolidWorks, they set up lower and
upper limits for what they figured CAD designers will actually deal with,
and it looks like a 500D arc is close enough to a straight line to not have
been woth the trouble to program for. There was actually an interesting
thread here about a month or two ago that discussed some other silly
cutoffs.... you might want to take a look for those old posts.
These internal cutoffs occur at the small end of things too, on some stuff
that I wouldn't characterize as being all that small... .004" is a
dimension that causes problems with the internal cutoff on some operations,
but it sure isn't an unrealistically small dimension for real-world
objects.
Call up your VAR and get them to think SolidWorks inability to handle your
circle is a bug, you'll get some nice internal results - and of course, do
the enhancement request thing too.
jp...@fast.net.au wrote in article <839s36$8lb$1...@nnrp1.deja.com>...
jaco...@my-deja.com
I do not think of this a build in limitation of SolidWorks, for I have
use it since its first version SolidWoorks 95, and I have never met
similar problem like you just mensioned.
Try to contact your reseller or log into SolidWorks subscription
website for further information or help. Or download the most currently
software upgrade.
Jacob
In article <839s36$8lb$1...@nnrp1.deja.com>,
jp...@fast.net.au
jaco...@my-deja.com wrote:
> After reading your mail, I believe you encountered a strange problem.
> I do not think of this a build in limitation of SolidWorks, for I have
> use it since its first version SolidWoorks 95, and I have never met
> similar problem like you just mensioned.
>
> Try to contact your reseller or log into SolidWorks subscription
> website for further information or help. Or download the most
currently
> software upgrade.
>
> Jacob
>
I have been using SW 99, time code 313.
In the main time I have been re-assured by my VAR that this _is_ a
built in limitation of the software. (The same, which does not allow
using bigger than 1000 units size entity through an input box. The
strange part of it is only the way it shows in this case.) They
suggested to put forward an enhancement request.... No comment.
Just another interesting thing: inbetween another VAR sent me a very
nice private letter, trying to prove that this is _not_ a real
limitation. He also attached a screen shot showing some circles on a
SolidWorks screen, bigger than those in question.
Well, I also know how to edit the dimension properties. But using this,
that certain circle does not get any bigger...
This much about the trustworthiness of a few "officially" looking
information on this newsgroup.
nich...@my-deja.com
quickly that you go back and re-read Ed Eaton's
previous post which is part of this thread. About
a month or so ago a post that Ed was part of
confirmed the fact that their does appear to be
high and low limits in SolidWorks. Use the search
capabilities in Deja. Once you find that post you
will be able to duplicate what was suggested in
the post.
In article <83ahh3$nb2$1...@nnrp1.deja.com>,
jaco...@my-deja.com wrote:
> After reading your mail, I believe you
encountered a strange problem.
> I do not think of this a build in limitation of
SolidWorks, for I have
> use it since its first version SolidWoorks 95,
and I have never met
> similar problem like you just mensioned.
>
> Try to contact your reseller or log into
SolidWorks subscription
> website for further information or help. Or
download the most currently
> software upgrade.
>
> Jacob
>
wro...@my-deja.com
copied a response from Ed Eaton's thread, although it is not written by
Ed. Wouldn't it be nice if a page in the documentation was devoted to
this sort of thing like they do in my HP calculator manual. Anybody that
wants to add to this table feel free. Does anyone from SWX want to add
anything?
Limitations:
Upper length limit: 1km (39370.0787402 in.)
Upper diameter limit: .5km (19685.0393701 in.)
Lower length limit: .001mm (.0000393700787402 in.)
Lower diameter limit:.002mm (.00007874016 in.)*
Lower limit on dimension from pierce point: .1mm (.00393700787402 in.)
Resolution limit: .001mm (this is the range of size of feature in which
SW can't make up its mind where it is and so may or may not fail in
making a feature.)
Note: When working with features near the upper or lower limits SW may
or may not be able to perform functions such as trimming which require
SW to resolve geometry past it's limits. EXAMPLE: Make two .002mm DIA.
circles and dimension .001 mm apart. Now try doing a trim. You will get
an error.
* You can make a circle .00199 mm in diameter, but I expect SWX thinks
it is really .002 mm in diameter.
The following is a quote:
SolidWorks apparently has built in limits on the maximum and minimum
size of features. The maximum size any feature can be is approximately
39,370.078 inches or .6214 miles. The minimum size any feature can be is
approximately .000039370078 inches. The number 39.37 is the conversion
from meters to inches. Most of you are scratching your heads and
wondering why be concerned about this. We don't design parts 5/8ths a
mile across or smaller than a tenth of a mil. I have tried using
SolidWorks for a civil engineering project and found the upper limit to
get in my way. If I was setting up an FEA of something on the scale of a
micro chip the lower limit would get in my way.
Ed Eaton found another limit. In dimensioning from a pierce point the
lower limit for the dimension is .004 inches. Go lower than this and
errors arise when creating a sweep.
I have found a related lower limit when trimming flush near a lofted or
swept surface. Trimming closer than .004-.005 produces errors.
SWX documents a similar phenomenon in creating a thread on a helix. They
state that at the root of the thread material should extend well into
the shank in order to avoid the "failed to merge bodies" error. My guess
is that "well into the shank" could be interpreted as greater than .004
inches.
Have any of you folks been able to confirm these limits or have you
found other limits? I would be interested to see what the SWX folks
watching this newsgroup have to say.
How would I model a feature 5 miles across? Is there any hope for user
control of tolerances and limits? And finally is anyone aware of similar
limits in SolidEdge, Pro/E or
UG?
P.S. The following was my response to Ed Eaton's posting.
Ed,
I haven't checked this out yet but here goes.
As you are probably aware SWX works in metric and converts to English as
a convenience. .004in is greater than .000393701 or .1 millimeters. This
magic number (393701) appears many times in sweeps, fillets, shelling,
lofts, etc. The .0003937 number is probably an arbitrary tolerance the
software engineers put in. I wish we could change tolerances. And I even
more strongly wish SWX would document the darn things. .1 mm is a rather
large tolerance.
Your discovery along with many other phenomenon I have seen suggest that
the real key to making SWX work is to know where these buried tolerances
are and what their values are. It is also a fundemental problem with SWX
in the sense that it prevents working close to edges that have been
created by lofts or sweep because SWX can't find the edge.
A further implication of your discovery is that SWX prevents you from
working on small parts. Suppose I want to design a nano-machine and do
FEA on it. If my nano-parts are .005 across the largest dimension I am
SOL.
Jay Guthrie
detailing a part that I needed a .00007 dia hole.
The stupid software wouldn't do it. The machinist were disappointed that I
made them drill a .00008 hole because my cheap software wouldn't work. They
like challenges and get bummed out when they have to drill them big fat
holes.
Jay
wro...@my-deja.com wrote in message <83o7vr$te9$1...@nnrp1.deja.com>...
zam...@my-deja.com
Does anyone know if this problem also exisits in SolidEdge or other
parasolid based mechanical design softwares? Could this be a kernal
limitation?
wro...@my-deja.com
Believe me, people run into these limits more often than you might
think. They weren't discovered just because somebody didn't have
anything to do.
When you get a "Failed to Merge Body" error, more likely than not one of
these limits is to blame.
In article <s60aim...@corp.supernews.com>,
R.H. (Rick) Mason
<zam...@my-deja.com> wrote in message news:83q7o9$b0n$1...@nnrp1.deja.com...
> Hi
>
> Does anyone know if this problem also exisits in SolidEdge or other
> parasolid based mechanical design softwares? Could this be a kernal
> limitation?
I just modeled a 12km x 6km block in SEv7, then put a 20km rad on
one side. SE happily accepts km as an input unit, just as it does
feet, inches, metres, mm etc.
R.H. (Rick) Mason
MASCO Design Services Pty. Ltd.
Solid Edge Support (Australia)
Sydney, NSW
Robert Berger
I'm curious what are you designing that needs a 0.00007" D hole? That's small!
What process do you use the create a hole that small and what type of tolerances
can be held?
:-)
Robert Berger
Chris Halasz
designed in Pro.
They needed the hole to transmit some infrared signal through the
bulwark -- to connect their Linux system calculating when to jibe.
Where did I read the draft angle on the hole in the blow molded bulwark
is 0.0000001 degree?
Robert Yule
all CAD software period. It always has. How you reach these limits is up to
the programmers and the math behind the model. I certainly don't understand
all the nuances of the solid modeling kernel math and this is a debate I
don't think any of us who need to produce parts wants to get into.
Many of the accuracy issue are also related to the relation of the largest
feature to the smallest feature in the model, So yes you may be able to
create the earth as a model, but can you then drill a .000008 hole in it.
I am an ex Pro/E user and can say that I used to run into the limitations
in Pro/E faster than in SW. Pro/E has a default resolution of .0012
(relative to what I am not sure) and I have had many cases where I would get
failed geometry with fairly simple geometry. I used to do a lot of thin
wall stuff (.012 - .015 typ) and it would often fail on cylinders of 3-4 in
or less. I often had to increase the resolution to .0001 (the max) to
regenerate.
Here is a simple test I discovered to get a feel for the accuracy or limits
of a modeler relative to each other. Create a cylinder 10in in diameter. Put
a hole in it (concentric to the cylinder) at 9.99 in. increase the size
toward 10 by 9.999 then 9.9999 etc.. You will find Pro/E fails at 9.997 at
.0012 resolution and 9.9997 at .0001 resolution. SolidWorks fails at
9.9999999 (although it leaves the cylinder - Pro/E you get the dreaded
failure screen). I need someone to explain to me so that my feeble brain can
understand how this makes Pro/E a more accurate modeller !
Also I have encountered situations in Pro/E where I have needed to increase
the accuracy to get a better IGES file (no open bits) only to have rounds
fail at the higher resolution. Pro/E is full of special case handling
routines where it allows things that it shouldn't from a mathematical point
of view. I have often got the message in Pro/E "case not supported" . Non
manifold geometry is a good example of bad (debatable) geometry will be
allowed in Pro/E - a tear edge in Pro/E sheet metal is where it will occur.
Parasolids does not allow non manifold geometry - which is a mixed blessing
! It means importing some parts from other systems will result in invalid
bodies, however it can save your ass down the way in that the bodies allowed
are always correct and will create good parts. One case handling I wish SW
would handle is when you want to create a sweep around a cylinder (a helical
cut for example) and you have to create your sketch geometry beyond the
silhouette edge so that it doesn't leave a gap (this was a problem in
original Boolean modelers). I got a good explanation of why it is so
mathematically but that doesn't make feel any better (by the way even with
the little extra geometry a helical cut in SW is soooooo much easier that
Pro/E).
I have a feeling that this discussion is the same discussion we used to have
with 3D wire frame and then surfaces. In wire frame (even 2D) if you had a
square of 1in for example, and then added a fillet to each corner and then
did a check on the end points they were no longer 1in (relative to the
opposite side) they would be .9999998 or something bizarre. This was always
due to the introduction of pi into the geometry and could result in open
gaps when translated. I saw this phenomenon on Unigraphics, Control Data
ICEMDDN, Cadkey, CADDS 5 and especially AutoCAD. The quality of the IGES
translation would also play into it.
All of these inaccuracies of all of the CAD software programs are why
companies that make geometry correction (e.g.. CAD Fix) a business can have
a business !
This thread also reminds me of when pocket calculators first came out (TI -
58 era) and the pocket protector crowd would stand around and bemoan decimal
place envy !
The bottom line is you need to be able to make parts and assemblies and have
models that can be manufactured. Whatever tool can do it is what is
important.
Cheers
Rob Yule
zam...@my-deja.com wrote in message <83q7o9$b0n$1...@nnrp1.deja.com>...
>Hi
>
>Does anyone know if this problem also exisits in SolidEdge or other
>parasolid based mechanical design softwares? Could this be a kernal
>limitation?
>
Robert Heininger
at a gnats ass on the moon!
Robert Heininger
Don Jackson
Don Jackson
kellne...@my-deja.com
That is a very interesting test. The other thing I have come across in
Pro/E is it's propensity to change dimension values during regeneration.
It used to drive us nuts. I have never seen SolidWorks do this.
Your test is a very good one. I just did a takeoff on it. Maybe others
will try to duplicate it on other software.
Solidworks will make a 0.00200000000050mm through hole in a .5 km OD
cylinder face, but it will not make a .002mm dia. hole. The ratio is 500
million to one, but the limits are absolute so as one works near one of
these limits the ratio goes down. For practical problems the ratio may
range from 200 to 200000 to one from the lower limit.
If anyone out there has Pro/E, UG, SolidEdge, IronCAD, MDT, Cimitron,
Anvil, or any other solids capable CAD package (or CAM for that matter)
run the following tests and forward the info on to me along with all the
usual stuff like your name, software name, version, etc. If I get the
data in time to compile it I'll bring it with me to New Orleans and
share it with you. After New Orleans I'll post it here.
Extrude a cylinder with a diameter and length as large as the software
will allow. In order to determine this you will have to slowly zero in
on a number to as many decimal places as you have patience for. In
SolidWorks this is .5km OD x .5km long. (As a side note mass properties
makes this cylinder 440.9 lbs heavier than it should be with a unit mass
although the difference is in the eleventh decimal place.)
Place a blind hole in an end face and dimension the blind hole along the
horizontal axis so it is offset from center. There are now three
variables, hole diameter, hole eccentricity, and hole depth.
1. With eccentricity set to zero and depth set to make a through hole,
decrease the hole size till it fails. Record results.
2. Slowly increase hole size till it works. There will be overlap
between step one and this step if small enough increments are used.
Record size at failure in the going smaller direction and size for
success in the going up direction.
3. With the hole set at the smallest size as determined in step 2
increase eccentricity of the hole till it fails near the edge.
4. Slowly decrease the eccentricity till it works again.
Record size at failure in the increasing eccentricity direction and
again in the decreasing eccentricity direction.
5. With the hole at the dimensions found in step 2 and 4 cause the depth
to approach the other end of the cylinder (it is not a through hole
anymore) till it fails.
6. Slowly decrease the depth till the part works again.
Record the size at failure going deeper till failure and then again
going shallower till success.
This data should give a pretty good idea of what the limitations of the
software are.
Robert Berger
I think what you are running into here is not a Solidworks limitation, but the Dynamic Range of the Parasolid modeling kernel. By dynamic range, I mean the smallest and largest difference between any two coordinates within a model space. I am familiar with what ACIS's limitations are in this area (Inventor, MDT, Cadkey, IronCAD and Vellum Solids). Practically speaking, the dynamic range of ACIS modelers is 0.00001 to 1,000,000 ( or any other example of 1e-5 to 1e 4). The smallest feature will limit the largest feature (and visa versa). I am assuming that Parasolid has a similar limitation. So in your example of a 0.002 mm hole within a 500,000 mm diameter cylinder seems to be running into the dynamic range limits of Solidworks. Based on this example ACIS appears to allow for more dynamic range. In the same circumstances ACIS is capable of defining a 0.00001 mm diameter hole within a 1,000,000 mm diameter face.
The reason that modeling systems run into this limitation has to do with efficiently performing modeling calculations on double floating point numbers (usually 14-16 digits long).
- In the case of ACIS, all objects are represented as double floating point numbers which contain 14 to 16 digits.
- ACIS allows that 4 of the least significant digits be used as "round-off errors" that occur during a calculation.
Regards,
Robert Berger
kellne...@my-deja.com wrote:
Robert,
Sent via Deja.com http://www.deja.com/
Before you buy.
kellne...@my-deja.com
Robert Berger <rlber...@earthlink.net> wrote:
>
> --------------9E7DD9079D1911580A14F767
> Content-Type: text/plain; charset=us-ascii
> Content-Transfer-Encoding: 7bit
>
> FYI,
>
> I think what you are running into here is not a Solidworks limitation,
but
> the Dynamic Range of the Parasolid modeling kernel. By dynamic range,
I
> mean the smallest and largest difference between any two coordinates
within
> a model space.
...clip
It may be the parasolid kernal or it may be SolidWorks. The limits are
very much absolute though. .5km and .002mm for circle diameters. We
won't know that till someone with SolidEdge or UG takes up the
challenge.
BTW, thanks for the info on the ACIS kernal.
John D. Ayer
I just tried and I sketched a circle with a diameter of 1000 meters in
SolidWorks.
It is my understanding that SW does have a limit of 1000 meters but I can't
tell you for sure.
Truthfully I cannot conceive of needing a part longer then 1000 meters. But
this is what I did to create one.
I sketched a circle 1000m in diameter. I extruded a base 500m. I extruded
a second boss 500m. I extruded a third boss 500m.
I had a couple of funky things happen that I believe may be related to my
video card that I will test out on a different system when I get back to
work.
As far as I know you can't ship a part that is 1000m in length. You would
need to build an assembly of multiple parts in any case.
Is anyone out there actually building parts larger than 1000m. That is
parts, not assemblies. A plant would be an assembly. The floor of a plant
more then 1000m by 1000m would be poured in separate sections.
--
John D. Ayer
<kellne...@my-deja.com> wrote in message
news:842tbh$2an$1...@nnrp1.deja.com...
> In article <38639ACD...@earthlink.net>,
> Robert Berger <rlber...@earthlink.net> wrote:
> >
> > --------------9E7DD9079D1911580A14F767
> > Content-Type: text/plain; charset=us-ascii
> > Content-Transfer-Encoding: 7bit
> >
> > FYI,
> >
> > I think what you are running into here is not a Solidworks limitation,
> but
> > the Dynamic Range of the Parasolid modeling kernel. By dynamic range,
> I
> > mean the smallest and largest difference between any two coordinates
> within
> > a model space.
>
> ...clip
>
> It may be the parasolid kernal or it may be SolidWorks. The limits are
> very much absolute though. .5km and .002mm for circle diameters. We
> won't know that till someone with SolidEdge or UG takes up the
> challenge.
>
> BTW, thanks for the info on the ACIS kernal.
>
>
Paul B. Kellner
"John D. Ayer" wrote:
>
> Hi All:
>
> I just tried and I sketched a circle with a diameter of 1000 meters in
> SolidWorks.
>
What OS and version of SolidWorks are you running on? Also, what
graphics card are you using?
Can you send me the .sldprt file? I was not able to achieve a diameter
of more than .5km nor were others able to.
Paul B. Kellner
"John D. Ayer" wrote:
...clip
> Truthfully I cannot conceive of needing a part longer then 1000 meters. But
> this is what I did to create one.
>
...clip
Originally I tried designing a BMX track and ran into this limitation.
Of course a BMX track is not something you would normally ship in one
piece as it consisted of a very large pile of dirt. Had SWX been able to
do this I would have known how many cubic yards of dirt needed to be
moved.
Eventually the BMX track was built. I used the Caterpillar solid
modeling system. It took a day and 60 gallons of #2 diesel.
M.B.Stephens
"Paul B. Kellner" wrote:
Sounds like that system should be Y2K compliant!
jp...@fast.net.au
"John D. Ayer" <cad...@nospamfiberia.com> wrote:
> I just tried and I sketched a circle with a diameter of 1000 meters in
> SolidWorks.
>
> It is my understanding that SW does have a limit of 1000 meters but I
can't
> tell you for sure.
By creation, SolidWorks does not allow using input values equal or
bigger than 1000 (m as the biggest unit) and equal or less than 0.001
(for mm, being the smallest unit.)
> Truthfully I cannot conceive of needing a part longer then 1000
meters.
This is usually not a problem for lengths - or lines - because this
would be big enough a part anyhow. The problem is with arcs or circles
wich are needed to create a much smaller part as this upper limit,
because 500m radius or bigger is not out of this world anyhow. This has
not got to do _anything_ with the physical size of any part - this a is
geometrical limitation.
Just for comparison: SolidEdge Foundation goes well beyond the upper
limit of SW (I tried circles with radii of 12,000 m -12 km-) with no
problem. IronCAD does the same. For the lower limit, though, SolidWorks
seems to be doing the (relatively) best job: SE Foundation rejects
everything smaller than 0.01 mm and rounds everything to a hundreds
accuracy. IronCAD is very unfriendly here: it does not accept anything
smaller than 0.1 mm and rounds everything to one tenth accuracy. (Or its
"unit" funtcion is very cleverly hidden in its interface). Still, it
runs away happily with a "nil" value, which drives SW crazy.
And SolidWorks seems to be somewhat uncertain with its accuracy:
allowing 8 digit unit setting it sometimes rejects any better than 4
digits accuracy and mixes up the feedback in its entry box - quite
strange.
As to the kernels: This above says me that SW's upper limitation of 1000
_is definitely not_, but its lower limitation _might be_ the lower
limitation of Parasolid itself.
To the original problem: I know very well the input limitation of
SolidWorks, which does not allow using anything above 1000 units. This
is clear: try drawing a circle of say 450m radius, and spin up its
radius with the entry box: it stops at 500. That's it.
But - and this was the strange thing - try to draw a circle just by eye
bigger than this upper limit. Then SW does two different things (I could
not determine which one and when and why). Sometimes it allows drawing
this circle, but it shows it in bright yellow, then saying the usual
error message:...impossible geometry, returning to the original status"
or something like this. Sometimes it does allow to draw the circle, in
the normal sketch colour, no error message. Even the circle remains on
the screen up to the next zoom : but it is unaccessible, does not
highlight and can not be snapped to etc.(and disappears at the next
screen refresh And again, sometimes the circle can not be drawn at all:
no error message, no yellow line - but no line at all.
Janos Nemeth
J&P Design P/L
John D. Ayer
Surf into the web page.
No, I couldn't make a circle larger then 1k in dia. I have worked on a lot
of projects over the years, I still can't conceive of needing a part with a
length of 1k. That is a part, not a landscape or even architecture,
although I could do both by modeling smaller individual parts in SolidWorks.
SolidEdge is not a very good product, although it does have some good
features. I work a lot with imported IGES files, surfaces and Solids.
SolidEdge won't let me modify imported parts in an assembly. Once I create
a part in the assembly I can't mate another part to it. You can't import an
ACIS file into SE without a translator. If you think SolidWorks is
difficult to use with surfaces (I don't) then run for the hills rather then
open a surface file in SolidEdge.
By the way, I believe it is Pro Foundation and SolidEdge Origin, although I
can't be certain.
I don't know IronCad, I haven't evaluated it.
SolidWorks uses the Parasolid kernel but it also has the acis kernel, just
open the about menu.
I guess I don't understand the point of the discussion, are you saying that
you believe that a limitation of 1k diameter is inappropriate? Or that a
lower limit of 1/100,000 of an inch is inappropriate? I read the original
post you made and in it you claimed that you needed a materials handling
schematic with a diameter of 600 meters. Now you are complaining that the
radius won't go over 500 meters? Did you make a mistake in your original
post?
As for the input of over 1000 units I just checked and I can input over 1000
feet.
As for dragging a circle over 1000 meters I just tried that and the circle
kept snapping back to 1000m. (change the dim to driven).
I suppose that I could generate an excel spread sheet defining points on a
600 meter radius and then import them into SolidWorks as a curve. I could
convert the curve into an undimensioned sketch. This would give me the
schematic I would need, if this is a real project. As a mater of fact I
could create an excel spread sheet with equations that would create a curve
of any size diameter. I haven't tried this but I believe that SolidWorks
has a pretty big envelope (10,000 meter cube, I think) and I imagine that
since we aren't working with dimensions this would work. If you really need
to achieve something like this and you aren't just trying to find problems
with SWX I will be happy to help.
I did manage to replicate the yellow circle at an 8 decimal place dimension
with a diameter of .0.00135469mm. This looks like a bug but I will have to
check it out some more to make sure. I am not sure that it is an meaningful
bug or what the color means.
Is anyone out there actually creating parts smaller then .01mm (.0001
inches) in diameter or over 1 kilometer (3280'-10.079") in length? Is this
something that we as engineers/designers need to be concerned about?
--
John D. Ayer
<jp...@fast.net.au> wrote in message news:848phd$qe6$1...@nnrp1.deja.com...
> Janos Nemeth
> J&P Design P/L
>
>
Robert Berger
I don't know IronCad, I haven't evaluated it.
SolidWorks uses the Parasolid kernel but it also has the acis kernel, just
open the about menu.
:-)
Robert Berger
John D. Ayer
John D. Ayer
"Robert Berger" <rlber...@earthlink.net> wrote in message news:38682228...@earthlink.net...John,
I don't know IronCad, I haven't evaluated it.
I use IronCAD....What exactly would you like me to try?SolidWorks uses the Parasolid kernel but it also has the acis kernel, justNo, Solidworks does not use the ACIS kernel. They use Parasolid 11. Solidworks does use a ParaSAT translator made by GSSL that licenses a subset of the ACIS kernel. It also uses the ACIS Deformable Modeler which is licensed from Spatial Technology. IronCAD 3.2 uses both ACIS 5.3 and Parasolid 11.1 simultaniously.
open the about menu.:-)
Robert Berger
Robert Berger
I guess my point was that I was trying to correct the misinformation that you posted regarding Solidworks use of the ACIS kernel. The same goes with your claims about the relative sizes of PTC and Dassault? This seems to be a habit of yours. I hope that it doesn't extend into your professional life.
I disagree with your second statement concerning my postings. I believe that my response to this thread explained what Solidworks users were running into, the dynamic range of the Parasolid modeling kernel. I thought it was relevant to the original poster of this threads question.
"It can help inform people of differences between SolidWorks and other products from a naturally SolidWorks slanted point of view."
I think this sentence sums up what you are about. Its truly galactic in its stupidity. I could never have thought of it on my own, so thanks! It is my belief and hope that you are in the minority in this group. Most Solidworks users are open minded enough to have a frank and truthful discussion.
No need to respond, unless of course, your ego requires the "last word". Be my guest,
:-)
Robert Berger
"John D. Ayer" wrote:
Hi: The point of this discussion is: Limitation in SolidWorks? How does your post address that My post was specific to a previous reply. The idea of this news group is to help people who are using SolidWorks to accomplish their goals. It can help inform people of differences between SolidWorks and other products from a naturally SolidWorks slanted point of view. Do you have a point in your postings? I have attempted to find a single suggestion in any of your postings relating to the use of SolidWorks. You generally argue with people. Do you have a specific point in any of this? --
John D. Ayer
"Robert Berger" <rlber...@earthlink.net> wrote in message news:38682228...@earthlink.net...John,
I don't know IronCad, I haven't evaluated it.I use IronCAD....What exactly would you like me to try?SolidWorks uses the Parasolid kernel but it also has the acis kernel, justNo, Solidworks does not use the ACIS kernel. They use Parasolid 11. Solidworks does use a ParaSAT translator made by GSSL that licenses a subset of the ACIS kernel. It also uses the ACIS Deformable Modeler which is licensed from Spatial Technology. IronCAD 3.2 uses both ACIS 5.3 and Parasolid 11.1 simultaniously.
open the about menu.:-)
Robert Berger
Robert Heininger
>> "It can help inform people of differences between SolidWorks and
>> other products from a naturally SolidWorks slanted point of view."
>
> I think this sentence sums up what you are about. <snip>
And I think the following does, too:
~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
Forum: misc.invest.technical
Subject: Buying cracked software CD's
Author: John D. Ayer <cad...@nospamfiberia.com>
Hi:
As an Applications Engineer for an engineering software reseller
<snip>
~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
Just adding my $.02
Robert Heininger
John D. Ayer
>
> Robert:
>
> From what I
understand, Solidworks uses only Parasolids.
This is
incorrect. Solidworks uses the ACIS Deformable Modeler and also licenses
the ACIS kernel for Parasolid to ACIS
translation.
Regards,
Robert Berger <rlber...@earthlink.net>
Seems
like you can change your stance to take whatever position you
want. Most people only interested in arguing will.
What do any of your postings in this thread have to do with helping someone either overcome or workaround a perceived limitation in SolidWorks?
I see no point to your postings. You do present your opinions in an informed and professional manner. I just don't see what they have to do with the thread? I am sure you manage to either bully, shame, ridicule or BS anyone who disagrees with you....how does this provide a service to anyone?
John D. Ayer
"Robert Berger" <rlber...@earthlink.net> wrote in message news:3868BB36...@earthlink.net...
Robert Heininger
<insignificant bandwidth snipped>
Warning : Ready the Silo's : Contact the President. . . .
We are going to DEFCON 5!
John Ayer:
LIGHTEN UP and GET A CLUE!!
The only mis-information (sans the bogus sales tactics by PTC) posted
on this newgroup the past few weeks, has been posted by YOU, and the
results have been very entertaining!
:-)
Robert Heininger
John D. Ayer
should be avoided by serious SolidWorks users!
Bobby you really don't have a clue do you?
Precisely what mis-information? I imagine you enjoy destroying newsgroups
with garbage rather then trying to help people achieve their goals.
Precisely what point do you have in attacking me or my posts?
I haven't read any useful posts by you. I don't expect I ever will either.
The problem here is that some losers take reasonable problems, like modeling
very large parts, and try and turn them into slamming software or people. I
would really like to see this turn into a website where SolidWorks users and
prospective users can come and get real information and help, including me I
might add. I wouldn't waste my time trying to surf in here on a 56K because
of people like you. I have talked to a lot of people who really hate all
this slamming. Now I am lucky enough that while I am working in the evening
I can stop and write a nice note. Kind of neat actually.
You go to defcon 5, I am going to take my dog out for a walk and then get
some more work done. If you really want to continue to spam why don't you
take it to my e-mail and quit wasting everyone elses time.
--
John D. Ayer
"Robert Heininger" <mong...@iinc.com> wrote in message
news:38695B08...@iinc.com...
Robert Berger
John,
My apologies for getting a little off track here, but maybe we can get some people on track. Anyone can open the help menu and get the information you need on ACIS. SolidWorks licenses portions of it's software from Spatial Technologies. I would like to know where you get the idea that they have not licensed the ACIS kernel or that they do not use it especially when you have posted that they do on other newsgroups?
They do not license the ACIS Kernel....
They do license the ACIS Deformable Modeler, NOT the ACIS Deformable Modeling Husk which requires the ACIS Kernel...
"Spatial Deformable Modeler brings powerful, easy-to-use deformable modeling
functionality to non-ACIS applications. (Similar functionality is available to
ACIS-enabled applications through the ACIS Deformable Modeling Husk.)"Solidworks also licenses PARASAT Plus from GSSL as a SAT translator. GSSL licenses a subset toolkit from both UG Solutions and Spatial Technology (not Technologies...).
Using you're definition, CADKEY uses Parasolid......
My point in this thread is to help someone make an informed decision. Something I do every day along with helping people solve problems that they are having difficulty with. Your point is? Spreading mis-information? Accusing people who point out your......problems?
You're a lightweight...stay in the shallow end of the pool. My point in this thread is to help someone achieve a goal in SolidWorks. The first posting claimed that a diameter of over 500 meters could not be achieved. I achieved it and explained how I did it to help the user and to help other users understand the real limitations in SolidWorks. How do your postings address this issue? I addressed his problem again with a possible workaround for even larger diameters. How have your postings helped anyone?
I explained the concept of Dynamic Range. It has nothing to do with how big something is, it has to do with the relative size. of features within a model. I try not to explain "workarounds", I'll leave that to you. I was interested in explaining "Why" this happens. I have continuously offered solutions to problems. I intend on helping people to solve problems because I enjoy it. From your postings I believe that you enjoy arguing and spreading mis-information.
Gotcha games won't help you here. Any reader with half a brain can see through you. Are you a VAR or do you work for a VAR as an application engineer? What exactly is your relationship with Solidworks Corp.? Or are you just a user?
Robert Berger
John D. Ayer
John D. Ayer
"Robert Berger" <rlber...@earthlink.net> wrote in message news:3869E94C...@earthlink.net...
Jon Banquer
Both products look to me like they will be moving further behind SolidWorks
when SolidWorks 2K is shown in less than two weeks in New Orleans. No
doubt this cause's Bob a level of frustration, as he has felt that SolidWorks
has not been a leader as of late.
I fail to see where the work VDS put into having dual kernels in IronCAD
makes ANY real sense, despite Bob's assertions that it does. How does the
small benefit of dual kernels make up for IronCAD's utter lack of hybrid modeling
tools ??? Sorry, I just don't see it. Seems like a great marketing ploy, though.
No doubt there are some benefits but nothing compared to the time wasted by
VDS / IronCAD not developing hybrid capabilities (If indeed they can be added
after the fact...the jury is still out on this.)
In general I think the level of frustration by mid price range CAD users has reached
a very high level because :
A. Lack of hybrid tools.
B. Still to difficult to use in many ways.
C. Lack of presence by strong affordable CAID modelers. (Something Bob has told me
will become obsolete.... I could not agree LESS. )
Personally, I feel a level of frustration over Varimetrix VX Vision not getting the
technical attention that I feel it deserves. (Do they have a marketing plan ?? )
This has been a huge source of frustration to me because this product shows that
hybrid functionality can be delivered for a reasonable price. No one has come
close to this achievement.
Here's to hoping SolidWorks does, because I don't see anyone on the horizon ready
to deliver the goods.
jon
Robert Berger
My mother always told me not to pick on kids who ride the short bus but in your case I will make an exception. You keep saying the same things, but where is your information coming from?
Document it or shut-up.
The information concerning the ACIS Deformable Modeler is available for your entertainment at Spatial's website (www.spatial.com). The ACIS Deformable Modeler is for non-ACIS Applications. The ACIS Deformable Modeling Husk is for ACIS-enabled Applications.The information concerning PARASAT can be found at GSSL's website (www.gsslco.com)
The financial and business statistics concerning the relative size of each CAD company is available at their websites (Dassault, PTC, SDRC and UG Solutions)under investor relations. Statistics concerning the number of seats, annual revenue, net income and staffing are all disclosed in annual reports and financial press releases.
Nothing that I claimed is esoteric knowledge, but are pubically published facts. Its all available to the public and is plain as day to anyone who knows there "ass from their elbow" about the MCAD industry. I haven't seen what I would consider a useful post written by you and I have looked around.
Luckily for me, I don't have to live up to your high standards. I comment on posts when I feel I have something to add to the group (as you do...). I suggest that you filter or ignore my posts. Truthfully I believe that SolidWorks could rip out the Parasolid engine and run the acis engine (or any other).....as some other intelligent people have commented the ability of the software to accomplish the goals here is the important part, not the specific engine. Kind of like a race, the driver should get the glory and the engine should be respected.
Not only can they, but they already have. Solidworks was originally developed using ACIS Kernel but switch to Parasolid back in 1995 (prior to release).
Sounds like you get your info from other people who post and not necessarily from a reliable source. Get a clue, you are lost in lala land.
So far, you've called me names. You've asked "what's your point?" countless times. You've asked me to document my facts. You've told me that I'm lost in lala land. But after all of this wind on your part a few things still are true:
All I did was point out to the fact that these statements. Perhaps, this was my mistake. You seem to be very dogmatic and I should have let the issue drop. You change positions based on the direction of the wind and not based on accurate information.....as if the sales crap UG publishes to sell it's stock is reliable technical information.
- My original post was correct and relevant in explaining about the dynamic range of modeling kernels
- You were incorrect about your assertion concerning the size of Dassault Systemes
- You were incorrect about your assertion Solidwork's use of the ACIS Kernel
- Every question that you have asked me, I have answered
- Any question that I have asked you has gone unanswered
- You have not backed up any of your statements with any references
That so called "sales crap" is submitted to the SEC and is every bit as valid as the "sales crap" that other publically traded companies publish. Do you understand what it means to be publically traded? The concept of stockholders, auditing accountants and the SEC? Dave Murray in his post implies that if it were to come down to semantics SolidWorks could in fact be interpreted as licensing the ACIS kernel. I can accept that he firmly believes what he says even if that is not the information I have. He makes his point very intelligently, something you don't do.
There's no doubt that Dave Murray's a bright guy and an excellent contributor the this forum. As to my ability to make a point intelligently, I'll leave that to the rest of the forum to decide.
The bottom line is that Solidworks licenses the ACIS Deformable Modeler from Spatial Technology and the PARASAT Translator from GSSL (GSSL licenses technology from UG Solutions and Spatial). They do not license the ACIS 3D Tool Kit (e.g. The Kernel) or any of its Husks.
In fact the definition of "kernel" is broad enough that Cadkey could in fact be interpreted as using the Parasolid kernel. It's relative..... like bigger. You seem to think the only opinion or definition in this world that means something is yours. Get real and get accurate.
So does Solidworks use the Pro/E kernel? Under your distorted logic because they have licensed a Pro/E to Parasolid translator from GSSL they use the Pro/E modeling kernel. Point made....Checkmate I can back up my position in documentation available to any SolidWorks user. Go to help about. You change positions with the wind.....like the wind bag you are. Produce verifiable documentation on your point (which you can only guess at) or get lost.
Moronic, dogmatic flame bullys such as yourself do not intimidate me. I encourage you to go to the websites that I referred to above and spend a little time reading before you post incorrect information. BTW, I don't see under Solidworks help where Dassault is the largest CAD company...Oh, thats right, "you losted the article".....
:-)
Robert Berger
Robert Berger
Bob uses both IronCAD and Vellum Solids.
Both products look to me like they will be moving further behind SolidWorks
when SolidWorks 2K is shown in less than two weeks in New Orleans.
No doubt this cause's Bob a level of frustration, as he has felt that SolidWorks
has not been a leader as of late.
I fail to see where the work VDS put into having dual kernels in IronCAD
makes ANY real sense, despite Bob's assertions that it does.
How does the small benefit of dual kernels make up for IronCAD's utter lack of hybrid modeling
tools ???
Sorry, I just don't see it. Seems like a great marketing ploy, though.
No doubt there are some benefits but nothing compared to the time wasted by
VDS / IronCAD not developing hybrid capabilities (If indeed they can be added
after the fact...the jury is still out on this.)
In general I think the level of frustration by mid price range CAD users has reached
a very high level because :A. Lack of hybrid tools.
B. Still to difficult to use in many ways.
C. Lack of presence by strong affordable CAID modelers. (Something Bob has told me
will become obsolete.... I could not agree LESS. )
Personally, I feel a level of frustration over Varimetrix VX Vision not getting the
technical attention that I feel it deserves. (Do they have a marketing plan ?? )
This has been a huge source of frustration to me because this product shows that
hybrid functionality can be delivered for a reasonable price. No one has come
close to this achievement.
Here's to hoping SolidWorks does, because I don't see anyone on the horizon ready
to deliver the goods.
:-)
Robert Berger
Jerry Steiger
John D. Ayer wrote in message ...
Caution! This post contains absolutely no technical content what so ever and should be avoided by any serious SolidWorks User.Bobby:My mother always told me not to pick on kids who ride the short bus but in your case I will make an exception.
John,I think you need to cool off. I have been following this news group for about a year now and your recent series of attacks on Robert are some of the worst examples of net etiquette that I have seen in that time. Robert has gotten into some heated discussions with other users but has never stooped to your level. It appears to me that he has his facts straight and that you are flailing. Lighten up, before you find yourself killfiled by the serious SolidWorks Users you refer to above.Jerry Steiger
Don Jackson
I was getting ready to respond myself. You said it very well.
Don Jackson
John D. Ayer
Believe me I understand frustration. The projects I get are usually not the
easy ones.
I hope you are right about SW 2K being shown in New Orleans. It would be a
good place to do it. It has been a long time between releases this time,
and last time for that matter. SW has consistently released functionality
that has driven the market and I expect they will this time also.
As for the ACIS kernel I have heard an entirely different story from someone
I know and respect. If you want we can discuss it some time. As far as I
know SolidWorks has not documented exactly what portions of the ACIS kernel
they use and I don't believe they will. I agree with you that having a
system where the user chooses between which kernel to use is a waste. As
the performance gap between ACIS and Parasolid narrows it really doesn't
matter which one you use to create a solid what matters is the functionality
of the software. Both ACIS and Parasolid have strengths and I believe that
SolidWorks makes good use of both, whether or not it is only husks or skins
or the roots.
--
John D. Ayer
"Jon Banquer" <jbt...@mpinet.net> wrote in message
news:s6k774p...@corp.supernews.com...
> Bob uses both IronCAD and Vellum Solids.
>
> Both products look to me like they will be moving further behind
SolidWorks
> when SolidWorks 2K is shown in less than two weeks in New Orleans. No
> doubt this cause's Bob a level of frustration, as he has felt that
SolidWorks
> has not been a leader as of late.
>
> I fail to see where the work VDS put into having dual kernels in IronCAD
> makes ANY real sense, despite Bob's assertions that it does. How does the
> small benefit of dual kernels make up for IronCAD's utter lack of hybrid
modeling
> tools ??? Sorry, I just don't see it. Seems like a great marketing ploy,
though.
> No doubt there are some benefits but nothing compared to the time wasted
by
> VDS / IronCAD not developing hybrid capabilities (If indeed they can be
added
> after the fact...the jury is still out on this.)
>
> In general I think the level of frustration by mid price range CAD users
has reached
> a very high level because :
>
> A. Lack of hybrid tools.
>
> B. Still to difficult to use in many ways.
>
> C. Lack of presence by strong affordable CAID modelers. (Something Bob
has told me
> will become obsolete.... I could not agree LESS. )
>
> Personally, I feel a level of frustration over Varimetrix VX Vision not
getting the
> technical attention that I feel it deserves. (Do they have a marketing
plan ?? )
> This has been a huge source of frustration to me because this product
shows that
> hybrid functionality can be delivered for a reasonable price. No one has
come
> close to this achievement.
>
> Here's to hoping SolidWorks does, because I don't see anyone on the
horizon ready
> to deliver the goods.
>
> jon
>
>
>
>
>
>
>
>
>
>
>
John D. Ayer
John D. Ayer
"Robert Berger" <rlber...@earthlink.net> wrote in message news:386AA412...@earthlink.net...
Robert Berger
John,
Hi Bobby:I hope you've noticed that throughout this "flame", I have not called you "Johnny. Says something about each of us doesn't it?
Long post I didn't read it but I skimmed it.
Sounds like your M.O. Maybe some Ridalin my focus you a bit.... You really don't get it do you? Either get verifiable documentation on exactly what portions of ACIS SolidWorks uses or shut up. The Spatial Website does not discuss exactly what SolidWorks does with ACIS. Go read it your self
I'll make it simple enough for even you. Try doing a find file for these two files:I suspect that you'll find edsps110.dll and not kern51.dll. You want to know why? edsps110.dll is the Parasolid 11 modeling kernel and kern51.dll is the ACIS 5.1 modeling kernel (ACIS 5.2 = kern52, ACIS 5.3 = kern53 etc.). Only ACIS enabled applications will have the ACIS modeling kernel. Unlike Parasolid, ACIS is broken up into modular dll's. If you don't have kern5x.dll you don't have the ACIS modeling kernel. Period.
- kern51.dll - a 4,344KB application file
- edsps110.dll - a 11,560 application extension
You have no clue exactly how SolidWorks creates a model.
It appears that I know a bit more than you....(See Above) If you know that SolidWorks was originally built around ACIS what makes you think they ever took it out?
That was 1995. It was ACIS 2.0. They are using ACIS 5x based translators and the deformable modeler didn't exist back then. They don't wan't to pay double royalties. Nuf said...You seem to selectively choose to accept what I say when it suits you. Curious habit.... If you want to know what Dassault is bigger, better or first at surf into their web site.
Another one of your lucid coherent points. How relevant! By the way, do you know why you have to keep posting and acting as if you know what you are talking about
First off, I dont have to do anything. I choose to continue this thread. Although I am sorry to continue to feed a "flame" war (sorry group:-(...) I have decided allow to self destruct in front of the group. You seem to be a knowledgable Solidworks user and have recently posted some helpful posts. Back in the 10th post in this thread all I did was correct a statement that you made:
"SolidWorks uses the Parasolid kernel but it also has the acis kernel, just open the about menu."
No big deal, right? What's wrong with correcting someone? This place is about learning isn't it? At least for most participants it is. It was all down hill from there. I'm not looking to argue or to create enemys here.
My participation in this God awful thread has now come to an end. Feel free to respond, but I am done. I believe that all readers who has been unfortunate to have followed this juvenille squabble can clearly see where each of us are coming from. After 7 posts we both have been able to communicate our points. I truly apologize to all of you who have had to read this flame.
:-)
Robert Berger
Jon Banquer
Your correct, you don't look good in this thread. Having said this, I am
very well aware that it's not a one way street.
Do me a favor. Please read the private e-mail you sent me a month or so
ago when I was going at it with Markoski. Compare the personality assessments
that you make in this thread, with the one's you made of me in the e-mail you
sent me.
Perhaps you may notice a remarkable resemblance. It's my belief that there is
a lot you could do to convey yourself in a better manor and make your points.
jon
nich...@my-deja.com
you for finally backing away. This thing between you and John had gone
on long enough. I don't know what you do but I do know that John is a
SolidWorks reseller in Michigan. He should know better.
In article <386BEE82...@earthlink.net>,
Robert Berger <rlber...@earthlink.net> wrote:
>
> --------------D869E47AAD4B99994CBE9F74
> Content-Type: text/plain; charset=us-ascii
> Content-Transfer-Encoding: 7bit
>
> John,
>
> > Hi Bobby:
> >
> > I hope you've noticed that throughout this "flame", I have not
called
> > you "Johnny. Says something about each of us doesn't it?
> >
> > Long post I didn't read it but I skimmed it.
> >
> > Sounds like your M.O. Maybe some Ridalin my focus you a bit.... You
> > really don't get it do you? Either get verifiable documentation on
> > exactly what portions of ACIS SolidWorks uses or shut up. The
Spatial
> > Website does not discuss exactly what SolidWorks does with ACIS. Go
> > read it your self
> > I'll make it simple enough for even you. Try doing a find file for
> > these two files:
> >
> > * kern51.dll - a 4,344KB application file
> > * edsps110.dll - a 11,560 application extension
> --------------D869E47AAD4B99994CBE9F74
> Content-Type: text/html; charset=us-ascii
> Content-Transfer-Encoding: 7bit
>
> <!doctype html public "-//w3c//dtd html 4.0 transitional//en">
> <html>
> <body bgcolor="#FFFFFF">
>
> <p><font face="Arial,Helvetica">John,</font>
> <blockquote TYPE=CITE><i><font face="Arial"><font color="#3366FF">Hi
Bobby:</font></font></i><font face="Arial"></font>
> <p><font face="Arial">I hope you've noticed that throughout
this "flame",
> I have not called you "Johnny. Says something about each of us
doesn't
> it?</font><font face="Arial"></font>
> <p><i><font face="Arial"><font color="#3366FF">Long post I didn't read
> it but I skimmed it.</font></font></i><font face="Arial"></font>
> <p><font face="Arial">Sounds like your M.O. Maybe some Ridalin
my
> focus you a bit....</font> <i><font face="Arial"><font
color="#3366FF">You
> really don't get it do you? Either get verifiable documentation on
exactly
> what portions of ACIS SolidWorks uses or shut up. The Spatial
Website
> does not discuss exactly what SolidWorks does with ACIS. Go read
> it your self</font></font></i><font
face="Arial,Helvetica"></font>
> <br><font face="Arial,Helvetica">I'll make it simple enough for even
you.
> Try doing a find file for these two files:</font>
> <ul>
> <li>
> <font face="Arial,Helvetica"><b>kern51.dll </b>- a 4,344KB
application
> file</font></li>
>
> <li>
> <font face="Arial,Helvetica"><b>edsps110.dll</b> - a 11,560
application
> extension</font></li>
> </ul>
> <font face="Arial,Helvetica">I suspect that you'll find
<u>edsps110.dll</u>
> and not<u> kern51.dll</u>. You want to know why?
edsps110.dll
> is the Parasolid 11 modeling kernel and kern51.dll is the ACIS 5.1
modeling
> kernel (ACIS 5.2 = kern52, ACIS 5.3 = kern53 etc.). Only ACIS
enabled
> applications will have the ACIS modeling kernel. Unlike
Parasolid,
> ACIS is broken up into modular dll's. If you don't have
kern5x.dll
> you don't have the ACIS modeling kernel. Period.</font>
> <br><font face="Arial,Helvetica"></font> <i><font
face="Arial"><font color="#3366FF">You
> have no clue exactly how SolidWorks creates a
model.</font></font></i><font face="Arial"></font>
> <p><font face="Arial">It appears that I know a bit more than you....
(See
> Above)</font> <i><font face="Arial"><font color="#3366FF">If you
know
> that SolidWorks was originally built around ACIS what makes you think
they
> ever took it out?</font></font></i><font face="Arial"></font>
> <p><font face="Arial">That was 1995. It was ACIS 2.0. They are using
ACIS
> 5x based translators and the deformable modeler didn't exist back
then.
> They don't wan't to pay double royalties. Nuf said...You seem to
> selectively choose to accept what I say when it suits you.
Curious
> habit....</font> <i><font face="Arial"><font color="#3366FF">If
you
> want to know what Dassault is bigger, better or first at surf into
their
> web site.</font></font></i><i><font face="Arial"><font
color="#3366FF"></font></font></i>
> <p><font face="Arial"><font color="#000000">Another one of your lucid
coherent
> points. How relevant!</font></font> <i><font
face="Arial"><font color="#3366FF">By
> the way, do you know why you have to keep posting and acting as if you
> know what you are talking about</font></font></i><font
face="Arial"><font color="#000000"></font></font>
> <p><font face="Arial"><font color="#000000">First off, I dont
<u>have</u>
> to do anything. I <u>choose</u> to continue this thread.
Although
> I am sorry to continue to feed a "flame" war (sorry group:-(...) I
have
> decided allow to self destruct in front of the group. You seem
to
> be a knowledgable Solidworks user and have recently posted some
helpful
> posts. Back in the 10th post in this thread all I did was
correct
> a statement that you made:</font></font><font face="Arial"><font
color="#000000"></font></font>
> <p><font face="Arial"><font color="#000000">"SolidWorks uses the
Parasolid
> kernel but it also has the acis kernel, just open the about
menu."</font></font><font face="Arial"><font
color="#000000"></font></font>
> <p><font face="Arial"><font color="#000000">No big deal, right? What's
> wrong with correcting someone? This place is about learning
isn't
> it? At least for most participants it is. It was all down
hill
> from there. I'm not looking to argue or to create enemys
here.</font></font><font face="Arial"><font
color="#000000"></font></font>
> <p><font face="Arial"><font color="#000000">My participation in this
God
> awful thread has now come to an end. Feel free to respond, but I
> am done. I believe that all readers who has been unfortunate to
have
> followed this juvenille squabble can clearly see where each of us are
coming
> from. After 7 posts we both have been able to communicate our
points.
> I truly apologize to all of you who have had to read this
flame.</font></font><font face="Arial"><font
color="#000000"></font></font>
> <p><font face="Arial"><font color="#000000">:-)</font></font><font
face="Arial"><font color="#000000"></font></font>
> <p><font face="Arial"><font color="#000000">Robert
Berger</font></font></blockquote>
>
> </body>
> </html>
>
> --------------D869E47AAD4B99994CBE9F74--
John D. Ayer
"Robert Berger" <rlber...@earthlink.net> wrote in message news:386BEE82...@earthlink.net...
wro...@my-deja.com
In your 12km x 6km block, what is the smallest hole you can put in it?
Once you have determined the smallest hole, what is the largest
dimension you can use to position the smallest hole?
Also, were you able to find and upper limit on the size of a feature at
all? 9E380km maybe?
> I just modeled a 12km x 6km block in SEv7, then put a 20km rad on
> one side. SE happily accepts km as an input unit, just as it does
> feet, inches, metres, mm etc.
>
> R.H. (Rick) Mason
> MASCO Design Services Pty. Ltd.
> Solid Edge Support (Australia)
> Sydney, NSW
wro...@my-deja.com
In a previous branch of this thread the question was asked: What is the
largest and smallest cylinder that can be made in various CAD packages.
There was even a listing given of what these limitations appear to be in
SolidWorks.
Try this test:
1. Find the largest diameter cylinder that can be produced in your CAD
package.
2. Once you have found the largest diameter, find the greatest length to
which it can be extruded.
3. On the end face of the largest, longest cylinder create the smallest
through hole possible.
4. Once you have found the smallest through hole, dimension it from the
center of the cylinder face and see what the largest dimension is.
Try Robert Yule's test:
1. Create a cylinder (any reasonable size).
2. Create a centered cylidrical through hole on the face of the
cylinder.
3. Increase the diameter of the hole till it fails. You may want to go
very slowly here because there may be a tolerance involved which causes
it to fail or succeed depending on which direction you approach the
number from.
4. You may want to vary the size of the cylinder and see it the
thickness of the remaining cylinder changes with absolute size or
dynamic size.
Hopefully several people with IronCad and other software will try this.
> I use IronCAD....What exactly would you like me to try?
Charles Bliss
from Inventor:
Largest Cylinder: 50,000 Feet
Extrusion: 3,280 Feet
Smallest hole in center 0.0000025 in
I created the extrusion in feet since it would get me to big quickly and
defaulted the hole to inches. I can think of no practical purpose for this
solid. At that distance, it didn't let me place a dimension between the
center of the hole and anything.
wro...@my-deja.com wrote:
Seth
"Paul B. Kellner" wrote:
> "John D. Ayer" wrote:
> ...clip
> > Truthfully I cannot conceive of needing a part longer then 1000 meters. But
> > this is what I did to create one.
> >
> ...clip
>
> Originally I tried designing a BMX track and ran into this limitation.
> Of course a BMX track is not something you would normally ship in one
> piece as it consisted of a very large pile of dirt. Had SWX been able to
> do this I would have known how many cubic yards of dirt needed to be
> moved.
>
> Eventually the BMX track was built. I used the Caterpillar solid
> modeling system. It took a day and 60 gallons of #2 diesel.