Modeling for FEA or Manufacturability? 1

[MadMango]

Many times we are required to model parts and assys so they can be manufactured with the least ammount of non-conforming parts. Sometimes this requires parts to bypass tolerances, and just be shorter/wider that normal. This means many parts in weldments have some large gaps (.06-.12in) that get fill-welded.

When it comes time to perform FEA, many of our assys fail the mesh sequence due to these gaps, and users are forced to add material back into parts to make faces touch. These gaps prove too difficult for SW weld beads handle most of the time, and we create in-context bits to fill the gaps to make a model for FEA work.

I'm wondering how other users handle this type of situation. Please share your work arounds, methods and solutions, as I'm sure I'm not the first to encounter these, nor will I be the last.

Do you create 2 models, one for FEA and one for Manufacturing?
Do you create simplified parts to represent your assys for FEA?
Is there something I'm missing?

Ray Reynolds
Senior Designer
Read: faq731-376
"Probable impossibilities are to be preferred to improbable possibilities."

 

[macPT]

MadMango

This is a subject not easy to deal and I think there's not an ideal solution (some times there's the need to change the strategy from one design to another).

Regarding welds, only in very special cases I create weld parts(when the absence of the weld gives a very wrong aspect to an assembly). But in these cases I never use SW weld feature: like you, I create incontext parts (it's much more easy to handle).

The normal process to represent welds is create the parts with their theoretical dimensions, give the necessary details for joint preparation (in part drawings)and, in the assembly drawing, I represent the welds using the ISO symbols.

For FEA I have a different procedure. I don't use welds or in-context parts. I've found that these can be very hard to manage by the FEA software (and it's one more part to process). I copy the parts and assembly to a different folder. In this folder I modify parts and mates in order to always have touching faces in places where a weld is expected. This way FEA can, by default, consider these touching faces bonded.

Another thing: I discard all details and parts that are not directly related to the part/assembly strength. Be carefull to not discard a detail that can be the key for assembly failure. First, try raw rapid analisys to predict behaviour and to decide which parts and details can be discarded. This way FEA is faster, more simple to manage, files are smaller and the probability of failed meshes or solving is lesser. In the end of the analisys I zip the folder contents toghether with the FEA files for future reference.

Hope this helps.

 

[TheTick]

Short answer: Yes, you will need a second model in many cases.

The idea of complete interoperability between CAD and FEA is still a fairy tale, no matter what your VAR may wish you to believe. Most such claims are made by folks who understand little about either design or analysis.

Is this a failing? I don't think so. Products are designed to be manufactured, sold, and used, not just to be tested. Changing CAD geometry to expedite FEA is no different than sanding off a little paint to attach a strain gage or drilling a small hole for a temperature probe. Just one of the many "shop mods" necessary when proving a design.

The needs of the analyst can differ greatly from the needs of the designer. There are many ways an analyst may need to alter geometry. Some of the points have already been mentioned, notably gaps, welds, and simplifying geometry. It is quite common to have to alter models before importing geometry into FEA software. Generally, I find CAD is the best place to do this, as most FEA softwares' geometry modeling capabilities are more limited.


You don't fight destiny, no sir... and you don't eat crackers in the bed of your future!

 

[TheTick]

You can expedite mods to SW geometry for FEA purposes by using the "Face-->Replace" and "Face-->Delete" functions. These can be real handy for simplifying geometry and closing gaps. Especially useful in dealing with imported "lump" bodies.

You don't fight destiny, no sir... and you don't eat crackers in the bed of your future!

 

[macPT]

TheTick

Some years ago (about 10!), I used Algor. It was (and I believe it still is) a very good FEA for PC. But there was a problem: the geometry needed to be created in it's own modeler, already is a mesh form (Algor had, at that time, a 2D mesh genarator and was introducing a 3D mesh generator, for which a didn't have a license). This was a bit painful and time consuming. If there was the need to change the mesh... you can only imagine how difficult it was. But once the geometry created, it was a very good FEA with lots of routines to control the model, change properties (we could even change properties, like stifness, in particular nodes!) and also a lot of informations in the pre and post processing files (much more powerful than the actual Cosmos!).

But I think that, although you are right ("interoperability between CAD and FEA is still a fairy tale&quot, the actual status it's better, even if you need to do extra work in your model so it can be used in FEA.

By the way, I miss alot those Algor tools for model manipulation and ASCII output files!

Does anyone knows such tools for Cosmos?

Regards

 

[bobsheets]

We all design different types of products, but I find it inconceivable that anyone could know enough about a body even less an assembly to constrain it or load it properly without using successive simplified models. I too have used Algor since the 386 Hyper days with "VisiCad" to model with. Even though we now design using solids I still find it necessary to build successively more complex models for analysis to verify the "assumptions" I must make.

Weldments are the most problematic of the structures we analyze. The assumption that all plates will behave like a casting can very often lead to skewed results. Using Plate or Shell elements in an Algor wire frame model allows us to limit the connectivity between plates to get the model to correlate with the physical unit in test. Without this correlation and an understanding or the sensitivity of the variables that control it the FEA can be very dangerous. The power of the dithered display never ceases to amaze me!

I have blasted SolidWorks for its recent inclusion of COSMOS Express in 2003. As a design department manager I think this feature should have been an install option. FEA like anything else can be a powerful tool when used with experience, skill and training, but in the hands of the ignorant it is very often wreck waiting to happen.

 

[macPT]

When I am referring to Cosmos, I mean CosmosWorks, not CosmosExpress.

There's already another thread that discuss CosmosExpress.
bobsheets opinion is very much in accordance with the general opinion in that thread, about how useful and how dangerous CosmosExpress can be.

bobsheets:
Do you still use Algor? Do you use it with SW? What is your opinion about actual Algor and SW connection?

Regards

 

[josephv]

Hello Ray,

We use configurations. We typically have an FEA configuration that is simple. We also have a configuration called ASSEMBLY, for our large assemblies (here we suppress cosmetic fillets, extruded text and detail).

cheers,

Joseph

 

[bobsheets]

My post was not to comment on COSMOS Express, that just slipped out. Sorry, lots of emotion there.

I use Algor with SW in the rare occasion I need a brick element model. With the InCAD extension to Algor the transfer is easy. Algor has done a lot of work to try and emulate the interoperability that COSMOS has naturally, its called FEMPRO. I can’t comment on COSMOS at all, I’ve never even looked at it. I have so much time with Algor I would not think of switching.

 

[TheTick]

Generally I find it's better to save off models as they go to FEA than to save a configuration. I do not want all the additional data following the part past its production release.

 

[macPT]

I also don't like to use configs. They are reserved for designs that are actually production variations of parts/assemblies.

I think that saving the files in another folder gives you more fredoom to do the necessary changes for a successful FEA.

As I already mention, in the end I zip these folders toghether with the related FEA files and archive the zip file in a CDROM. This way, if needed, I can retrieve the model and FEA solution. The files in the server (the production files) are not oversized with data not needed for production purposes.

Regards

 

[MadMango]

Thanks for the input folks. We were planning to do as macPT, and create an entirely new set of assys and parts (in a new sub-folder), and modify them for FEA work, then archive to CDROM. I just wanted to see if others came to the same solution.

TheTick, first off... "Spoon!!" Thanks for the suggestion about Face> Replace/Delete, I'll try that when I get a chance.

For areas that are interval/stitched welded together, do you just make the faces coincident, or do most people add in the individual welds? For example, I have 2 L-brackets placed together to make a rectangular tube with a flange, like this:
|----|----
|____|
This is interval welded 1.00-4.00 down the it's length of 25inches. I know it's more accurate to simulate the welds for FEA, but it is worth the trouble to go to that extent, or can I just merge everything to give me a continuous face-to-face contact.

Ray Reynolds
Senior Designer
Read: faq731-376
"Probable impossibilities are to be preferred to improbable possibilities."

 

[EdDanzer]

During 1997-1998 we did a project where weld simulation in Cosmos was of great importance. SolidWorks provided a join feature to make the assembly a solid model. This as well as assembly modeling sounds good until you have a complex weldments. In the end we created solid models that were built with gaps between the pieces using a correctly sized weld bead to give models that represented the actual fabrication. Lapped plate parts have mill scale that separates the pieces, flame cut parts never fit tight, and fixtures have some variation, so leaving gaps will give the most accurate results.
Simplifying a weldments to make the FEA simpler will not work if it is a critical part. The problem with weldments is that the weld will become the start of fatigue if it is a loaded part. The weld area is a transition zone making a good design some what difficult to achieve, it will either be to stiff or to high of stress close to the weld bead. Having built and tested several FEA weldments to failure, only simplify if the model is too large to mesh. We tried an assembly FEA, had 60 hours of run time on the model when it failed, made a solid model, and ran the FEA in 30 hours total.
Don’t waste time saving the files created for analysis unless you save the version of SolidWorks and Cosmos, after a Rev or two comes out you cannot access theses files.