Skip to main content
scollins1-Visitor
1-Visitor
July 15, 2014
Question

less than impressed with Creo Sim 2.0

  • July 15, 2014
  • 18 replies
  • 5762 views

I've been trying to deal with a 20 pc. assy., but currently crashing. I cannot post pics nor assy/prt files. This is essentially a flat plate w/both simulated fasteners and solid screws into a fixed mounting structure. Plate has a pressure load applied. The fastener preload iteration took 8 hrs to run on 'quick check'...

 

I need this to RUN!!!!!!!!!!!!!!!!!!!!!!

 

At this point, no preload on the solid screws is necessary

 

I feel this has taken far too much time....approx. ~100k elements, (if I can even get it to complete the mesh).

 

To prevent chattering, I've tried to match tols by switching all part accuracies from 'relative' to 'absolute'. Using def. tol of 1e-4,

 

refined meshing on rounds, cbores, thru holes of interest...thru Autogem....used a lot of 'Max. Elem Size' and 'Exclude Singularties' @ re-entrant<150 deg.....

 

Nodes? I have laid down some of these - There seem to be directional arrows....right click in collection box and "fix"...did this....

 

Autogem Settings - "detailed fillet modeling" is checked...

 

There is a skeleton with curves I used to trace the sim region...this seem ok....

 

I've gone down to the part level and refined meshes there, am intending on using these piece part meshes at the top level...am I wrong to assume this?

 

How is it that I can't get this to kick, but every little demo and presentation is always just sunshine & smooth sailing....

 

 

Now - the ANSYS group is chomping at the bit to get their hands on this and I have no grounds to hold them at bay..I have until Fri. to get this assy. running...

 

btw- brand new M6800 w/32Gb...so it's not the hardware...

 

cpu 'use all'

 

Q: Comments? methods?

 

Thanks for your attention and review..

 

Sean


This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

18 replies

scollins1-VisitorAuthor
1-Visitor
July 16, 2014

Thanks for the response...yeah I thought this should be easier, if it's just the plate, no problem but a top assy not so good...chewing up a lot of time, will go to SPA. Yes..contacts...a number of them

The stresses in the plate & stress in simulated fasteners (10X) are my primary interest. Not interested in fixture stresses, mount is fixed in 3-dirs...also not interested in some fastened components..but I need them for the assoc. weight.

yes.. plate assy. is "screwed" to a fixture, so I can get fastener stresses...

addt'l info...

both plate & fixture are made of 2 materials, so I merged the plate into one .prt and fixture piece into one .prt to produce a 2 part assy. and be able to use simulated fasteners.

The solid fasteners are just there for contact, I bonded them to the fixture. Preload on these would be nice for completeness, but not necessary.

dschenken2-Explorer
2-Explorer
July 16, 2014

Best suggestion I can make is to sneak up on it. Use cuts to remove most of the geometry and see if one small piece with one fastener works. Move the cut back and see when it stops working right.

Had an Ansys failure with heat transfer - put in a million watts per square inch to get a .1F rise in temp on a tiny fin. Turned out Ansys never tried non-metric units with that module in their testing and it didn't work otherwise.

So. Convert the problem into one that is too simple to fail and work from there.

scollins1-VisitorAuthor
1-Visitor
July 16, 2014

I'm working on it now, messing with the Geo Tol...not having any luck.

Previously, I had suppressed piece parts and got it to run, albeit a long runtime, and I have suppressed chamfers, holes, rounds on various, but now I need the assy to run!

sdensberger2-Explorer
2-Explorer
July 16, 2014

Couple pointers that you can use to diagnois your problem:

  1. To help narrow down whether a meshing problem is due to a tolerance difference between components or due to geometry, suppress all interfaces that you've defined and change the default model setting to free. If the model meshes without a problem, then your issue is likely an interface one.
  2. It's generally best that you don't add in any mesh controls until after you've gotten your model to run.
  3. I don't know for certain (since I can't look at your model), but 100k elements sounds like waaay too many. Remember, Mechanica is a p-version FEA code; chunky elements with large aspect ratios (30:1) can still give very good results.
  4. I'm not sure if you're using solid geometry for your fasteners or if you're using idealized fasteners via the fastener tool in Mechanica, but if it's the former, then make sure that the fastener and nut can't 'spin' in place. This rigid body motion will result in a singular stiffness matrix.
  5. It's typically best to add in a couple components at a time, do your pre-processing work on them, mesh and run, and then add in more components.
  6. You can run a modal analysis with the rigid body mode box checked to see if any of your components are undergoing rigid body motion.
scollins1-VisitorAuthor
1-Visitor
July 16, 2014

Thanks Shaun,

yes...100k is wayy too many...

I had a simpler model running, added mesh control, then had to add components...then snags that I'm trying to get over.

I've been keeping the diagnostics box clear of edges/surface removals flags by modifying the Geo Tol. Settings.

I will double check the solid fasteners that they are set in 3-dirs.

I'm getting some degenerate surfaces

Sean

scollins1-VisitorAuthor
1-Visitor
July 16, 2014

suppressed the Autogems....back to crashing the program.

Thanks for you review and assistance..

Sean

scollins1-VisitorAuthor
1-Visitor
July 17, 2014

Better news...the top assy has run (SPA) ...attached are files...

I modified the Geo Tol FROM: 1e-4 & 0.86 deg. TO: 1e-3 & 1 deg., iterates faster now. Most Autogems are still suppressed.

Still can't get my 3 simulated "Primary" fasteners to come in...

was thinking...should Autogem limits be reduced and Geo Tol be increased?

Sean

346gnu13-Aquamarine
13-Aquamarine
July 18, 2014

A quick look

From the .rpt file

One immediate issue you have to look at ...

At the top of the .rpt file :

** Warning: Two faces (DBIDs: 83341938 & 83208508) on opposite

surfaces in a contact (DBID: 82855602) are

connected at a node (DBID: 82789300). This prevents

the surfaces from moving completely apart during

a contact analysis. If this is not what you

intended, please edit your model appropriately.

Probably means that the boundary of one of your contact regions is is attached to the opposite surface when it possibly should be free to slide/separate, This will mean load will be transferred through these nodes and the structure not move as it should. Local fastener forces will be affected.

One cause of this, for example, is the creation of a surface/volume region after the definition of a contact. The original contact now has to become 2 contacts and you only defined 1.

Review the run diagnostics, these will appear as orange dots. Select one and see what is highlighted in the model. You then have to reverse engineer the reason to fix it.

Ignore the following for now.

*** Warning: Large deformation and/or strain detected during contact analysis.

More accurate results may be obtained if 'Calculate Large Deformations' is selected.

Switching on LDA will cause a ramp up in analysis time you don't need at the moment. Besides, it could be inappropriate is material strains are low and the large movement is due to sliding.

The fastener forces. One shouldn't expect more than a few percent variation from preload values

Buffer# - 1.7e4 - ish ok?

Cylinder 312 to 2.3e4 - quite a range,,, suspicious

secondary - 712 to 1.6e3 ....mmmmmmmm

clamp3, insert1&2, promary4,5,6, secondary 3,5,6 small numbers, likely to be wrong (if these are fasteners).

tele# - all 7.5e3 -ish ok?

2. Causes of smaller than expected fastener tensions:

-Local contact region boundaries sticking to opposite surface (above)?

-Fastener surface regions (created by the software) running off the edge of a component/into tangent lines (rounds) overlapping neighbouring fastener regions.

Analysis time is reasonable.

From the .pas file, the residual norm 'collapses' in a well behaved manner, the contact solution seems good.

    Terms & ConditionsAccessibility statement