Creo Simulate - Element incompatibility

[rbowen]

Hi all,

Can anyone assist with  'Element Incompatibility' Issue?

I have inherited a model featuring fairly complex extruded sections of a frame.

I have checked geometries, interfaces and constraints in Creo Parametric 2.0 design, such that it allows me to enter Simulate with no error.

However, when I try to AutoGem the model, I obtain the error below, for certain curves (edges).

(Orange dot):

AutoGEM has detected an element incompatibility across the

highlighted curve.  Adding points to the curve may help.

In some cases, re-creating the curve and adjacent

surfaces may be required.

Does anyone know if there is a technique I can use to try and remedy this incompatibility , and what may be the root cause?

There does not seem to be anything fundamentally wrong with the design of the parts.

I tried to create a Modal analysis, but would not run either

Any adjustment to the parts would mean a significant assembly re design, but if I know which direction to go then it will be worth it.

Maybe certain Sections are not compatible with Simulate?

An example section (for which this error exists) is attached.

Such section is part of a large frame assembly, joined at mating faces.

Any advice appreciated. Many Thanks

[DenisJaunin]

Hello Richard,.

Have you checked all the characteristics, units, material of your room.

Could you contact the your part file if it is not confidential.

Kind regards.

Denis

[gfraulini]

Hi Richard,

have you tried to look at the "Geometry check" tool?

Usually are too many little surfaces left by successive cuts that generate them.

Can you attach the file?

[unickque]

My remedy for these type of issues is to cut away a tiny bit of material around the problem area, such that it will not impact the results.

[346gnu · Accepted solution]

Yup. and/or (not an exhaustive list)

First. Bring each component in 1 by 1 and mesh. Fix the failing components. Remember how many elements each component required.

• 'model over the top'. i.e. bury the offending feature under a new surface. (it doesn't have to be pretty, it simply mustn't affect you results significantly)
• place an Autogem control on the offending line/ part
• Examine the geometry where curved surfaces meet others at 0deg. Cylinders appearing out of flat plates where the cylinder is tangent to the edge of the plate. Manually adjust. (for cylinders, read curved surfaces)

With all components 'mesh-able' you are left with interface issues (you have shown that the parts are ok above)

Second. Add up the elements for all components. Your assy should have approximately this number. Significant deviation from this number will be due to small edges created by interfaces

In an assy:

• Ensure that fasteners' 'head' and 'separation' diameters are away from tangent lines, edges and each other.
• Contacts. Switch off 'split surfaces' if they are active.
• Check every connection for tiny overlaps and adjust so there are no very tiny overlaps/overhangs.
• Try and put assy level features into parts
• Change external rounds to be slightly larger than internal rounds where components meet each other (e.g. bearings into thrust faces). This separates tangent lines and can reduce number of contacts
• Adjust the accuracies of the parts such that tolerances are same order of magnitude as neighbours (use 'tolerance report' from within simulate)
• Overlapping volume regions can be troublesome

have fun

[anthonyws]

---

@346gnu wrote:

Yup. and/or (not an exhaustive list)

First. Bring each component in 1 by 1 and mesh. Fix the failing components. Remember how many elements each component required.

• 'model over the top'. i.e. bury the offending feature under a new surface. (it doesn't have to be pretty, it simply mustn't affect you results significantly)
•  
• place an Autogem control on the offending line/ part
•  
• Examine the geometry where curved surfaces meet others at 0deg. Cylinders appearing out of flat plates where the cylinder is tangent to the edge of the plate. Manually adjust. (for cylinders, read curved surfaces)
•  

With all components 'mesh-able' you are left with interface issues (you have shown that the parts are ok above)

Second. Add up the elements for all components. Your assy should have approximately this number. Significant deviation from this number will be due to small edges created by interfaces

In an assy:

• Ensure that fasteners' 'head' and 'separation' diameters are away from tangent lines, edges and each other.
•  
• Contacts. Switch off 'split surfaces' if they are active.
•  
• Check every connection for tiny overlaps and adjust so there are no very tiny overlaps/overhangs.
•  
• Try and put assy level features into parts
•  
• Change external rounds to be slightly larger than internal rounds where components meet each other (e.g. bearings into thrust faces). This separates tangent lines and can reduce number of contacts
•  
• Adjust the accuracies of the parts such that tolerances are same order of magnitude as neighbours (use 'tolerance report' from within simulate)
•  
• Overlapping volume regions can be troublesome

have fun

---

Haha, That's a doctorate level thesis. For the $$$ it should be robust enough to automatically asses these minor inconsistencies and make adjustments. Imagine attempting to analyze a bicycle wheel. every spoke would likely give errors. or a truss with many parts. Every time I use AFX to build anything I end up just going into the shop, cutting and welding the parts and loading it with weight to proof load it. much faster and more useful results than simulate with AFX. Rant over.
 

[rbowen]

Many thanks for all your advice, I will review model and post my findings.

Unfortunately I do not think I can release any parts at this stage; due to security issues.

Regards

Richard