Ansys 10 Multiphusics + Solidworks 2006

[AtResonance]

Hello everyone:

I am a beginner to FEA and have a Solidworks 2006 assembly that I am trying to work with in Ansys 10 multiphysics. My assembly is pretty simple with a dozen or so parts. I say it as a parasolid and use import to bring it into ansys, then the VGLUE, ALL command to have my volumes share the common boundries I believe from my mates specified in SW.

Here are my 2 questions:

1. When I do this I get an error of the form "line 274 on area 134 is not on the area within tolerance..." is this a terminal problem? What might be the cause?

2. What I see imported into Ansys is a wireframe (sort of) of my solid model...is this an import issue or am I really better off getting the SW plug-in for ansys to save me pain?

Thanks in advance for any help!

 

[Stringmaker]

Unfortunately it sounds like you have a poor quality CAD model or the allowable geometric tolerance within Ansys is very small. I can't remember what options Ansys gives when importing Parasolid off the top of my head but if there are any options which allow you to merge coincident points within a certain tolerance loosen that up a bit. Things like this typically default to 1E-5 in Ansys which is extremely tight for the default settings of most CAD packages. I'm in no way familiar with SW but here's what I would do:

1) Loosen up any import tolerances to merge points IF Ansys gives you that option with Parasolid or tighten the export tolerances if you can within your CAD package if possible.

2) Export as an IGES instead and import this into Ansys. This gives you a good number of import options. It's the CAD format Ansys handles best.

3) Use the NUMMRG command within Ansys to merge keypoints coincident within a certain tolerance. Try something like NUMMRG,KP,1E-3,1E-3.

Hopefully one of these suggestions will be of help. If you still cannot achieve a good clean model after trying these out some geometric repair may be needed on your part. Let us know how this works.

In regard to your question about wireframe make sure you're plotting either areas or volumes and enter /FACET,NORML in the command line. Most likely your setting now is /FACET,WIRE hence the wireframe.

Good luck,
-Brian

 

[Stringmaker]

Actually, on second thought before you try any of the suggestions in my first post try adjusting the boolean tolerance. For instance, BTOL,0.001 sets the tolerance to 1E-3. Don't get overly generous with this however.

-Brian

 

[AtResonance]

Thanks for the reply and help.

I am actually not sure that the direction I am heading in try to solve these errors is the best as I believe I've found that the VGLUE, ALL command "binds" together my 13 or so separate parts into a single volume...this is not helpful as I have multiple materials to specify and it would seem that I want the volumes separate to allow me to specify the individual properties. But be that as it may...the head banging I am doing along with the clues provided is moving me forward...so let me tell you the results from your suggestions:

1. BTOL, 0.001 followed by VGLUE, ALL - this gave me a new error: Boolean operation failed try adjusting the tolerance value on the BTOL command to some fraction of the minimum keypoint distance. Model Size(current problem)8.590153e-2, current BTOL setting 1.0e-3, minimum KPT distance 2.54e-5. I also tried BTOL, 1e-4 follow by VGLUE, ALL and got a different error. Again, though, I am suspecting that I shouldn't be trying to do a VGLUE, ALL as I think this should be used when you want to convert multiple volumes of the same material into a single volume?

2. Loosen-up tolerances on merge points in ANSYS or Solidworks...don't see how to do this in Solidworks not sure in ANSYS but again I think I was headed down a wrong path as I want my 13 volumes seperate and unique but with mating surfaces.

3. IGES or other formats for export/import. Tried these as well with less success than the parasolid...but similarly to 1 & 2 above I think I was headed in a wrong direction.

4. NUMMRG,KP,1E-3,1E-3 - This reduced my 13 volumes to 1.

5. On the wireframe vs facet...that was my problem! From the GUI selecting PlotCtrls -> Style -> Solid Model Facets... -> Normal Faceting, got me my solid model back and a degree of comfort my model isn't totally whacked now that I can see the individual volumes.

I really want to thank you for the suggestions as they have kept me moving forward. As a total newbie to ANSYS I have a couple of procedural questions maybe you could help me down the right road with:

Description: I am modeling a piezoelectric transducer with 13 parts(volumes) and ultimately want to be able to experiment with various geometries of the acoustical tips...12 of my 13 volumes will remain unchanged I'll just want to keep swapping out 1 part in my CAD package and in ANSYS. The 13 parts are comprised of 4 materials.

Problem: Each time I import a solid model into ANSYS it seems I must go through a lot of tedious work(define my 13 part materials, meshing, etc.) and since I'll be looking to run this model repeatedly with different tips...should I be looking into setting up a macro or capturing a script of the ANSYS commands? Right now as I am learning, I have to go through and redue alot of work each time I restart with a new model. Any suggestions on approach to using ANSYS efficiently?

Sorry for the long post but again thanks for keeping me going forward!

 

[Stringmaker]

The VGLUE command is only useful if you want volumes to share the same nodes at their points of interface and form a sort of bonded contact. Otherwise you won't find the command of any help. Ansys can be a real stickler when you import dirty geometry as you're finding out. Many times reducing the BTOL helps significantly. I don't use glue operations very often so I'm of little help there. I've read through your error messages and without actually having the model on my workstation it's really tough to diagnose your difficulties. I would talk to your ASD about your problems as they sound to be a little above the norm. Solid works should have some sort of tolerances which you can make smaller for part export which should help you significantly. Look into that or search the help. I know very little about SW.

As far as ways to make your job easier you can infact do this by using a macro. Stuff like this is where Ansys excels over GUI driven programs. What I would do is assembly a database with the twelve constant parts in it that remain unchanged for each analysis. For each different tip design you will want to have a seperate database. What you can then do is using the CDWRITE and CDREAD commands you can import the different tips into your main twelve part assembly. For assigning material properites, reals, etc forming elemental components using the CM command is very helpful for selection. For 95% my models the onlything that is done via GUI is meshing and geometric creation and editing. Everything else such as assigning materials, settting up contact, running the analysis, and even post processing I do via macro. It may seem like more work at first but typically saves time in the end. Most of our designs are iterative however and several iterations and many different cases are done for each. Plus making changes to an input file is very quick.

If you are using Ansys a lot you'll become a much better and more efficient user by doing things via macros.

Good luck,
-Brian

 

[AtResonance]

Thanks again Brian...

As for my model issues I think I will just let them play out as I continue with building my analysis...keeping them in mind as I go.

The macro path is what I expected and I just wanted confirmation that this is worth my time...I believe it is. I think I will pursue a macro for my twelve part assembly and then study the CDWRITE & CDREAD functions as you suggest...this should keep me plenty busy for a while.

I really appreciate the help is steering me in this general direction! I'm sure you will see me back in the not too distant future!