Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

Differences between Simsolid and Inspire for Modal Analysis

Hello,

I'm investigating different software tools for modal, and other types of analysis, with a focus on Design for NVH. I'll say I'm not "an analyst" but seem to be heading down that path somewhat.

At first, Inspire was used, as we have an Altair evangelist here and he recommended it to our design department. This didn't seem to have a complete set of tools but does to basic modal with a powerful solver in the back end. Next, I tried Simsolid as it seems to have more tools available for understanding NVH performance, while still being relatively easy and doesn't require full analyst level understanding and tools.

There seems to be quite a difference in the modes calculated, eigenfrequencies. The part I'm using is a three piece welded assembly that is fairly simple (essentially cantilevered beam) as far as welded sheet metal parts go. I believe I set up the constraints similarly, with grounded bolts in Inspire and immovable inside surface of the bolt holes in Simsolid and similar contacts where welded.

The major difference seems to be the first mode, being up to ≈16% different. The higher modes are typically closer, but some are ≈10% different, with most being ≈5% or less. I would accept 5% personally, but the first mode is concerning to me. When the solving settings in Simsolid are changed to 5 passes with high refinement, the differences are larger (lower 1st mode frequency, ≈20% difference) than when standard 3 passes with standard refinement is used.

Inspire is the more trusted result right now because our evangelist knows and trusts Optistruct solver. I liked that Simsolid has more analysis types available, but it is largely unproven here.

Short of building a part and testing it, does anyone have any experience with what solver is more accurate in general?

Any other feedback on maybe I didn't constrain it similarly like I thought or other potential areas for improvement?

Are there other recommended tools for NVH dynamic analysis types that would be better than these? Do I need to go all in on hypermesh, optistruct, others?

Simsolid vs Inspire.PNG

Find more posts tagged with

English

Inspire

SimSolid

Accepted answers

RobHoglund

Hi Ben,

In addition to what Chayan suggested, can you confirm if you ran the Inspire (OptiStruct) model with 2nd order elements? You may see a closer first mode than with 1st order elements.

Rob H.

All comments

Chayan

Hey Ben,

All things considered being the same, SimSolid and Inspire should give you results that are within 5% of each other. We have tested it out on numerous cases.

The differences in the model setup (Boundary conditions, contacts, materials etc) are the typical culprits for results not matching.

Take another look at the model, check the geometry to make sure that the contacting surfaces are properly touching each other, maybe increase the contact resolution in SimSolid, in case you feel the contact is not engaging completely.

I'm sure you are using the exact same material, but doesn't harm to check once more.

You could also run a free-free analysis to ensure that the BC's are not the issue.

Hope these help.

RobHoglund

Hi Ben,

In addition to what Chayan suggested, can you confirm if you ran the Inspire (OptiStruct) model with 2nd order elements? You may see a closer first mode than with 1st order elements.

Rob H.

Chayan

You are right Rob. I missed mentioning about 2nd order elements. The results from Inspire are stiffer compared to the the ones from SimSolid. That could indeed be due to using 1st order tetras and not second order tetras in Inspire.

Ben T

Hi Ben,

In addition to what Chayan suggested, can you confirm if you ran the Inspire (OptiStruct) model with 2nd order elements? You may see a closer first mode than with 1st order elements.

Rob H.

Thank you both for the advice!

I ran both solvers within Inspire, to guarantee same material and minimal differences with contacts. Once I forced second order elements using the "More accurate" and "Sliding with separation" radio buttons they were much closer, generally within 1-2%. The second mode was a little bit of an outlier at 7%, but I think I can live with this improvement to the first mode.

Is using 2nd order elements a best practice when doing modal analysis with Optistruct?

Chayan

Thank you both for the advice!

I ran both solvers within Inspire, to guarantee same material and minimal differences with contacts. Once I forced second order elements using the "More accurate" and "Sliding with separation" radio buttons they were much closer, generally within 1-2%. The second mode was a little bit of an outlier at 7%, but I think I can live with this improvement to the first mode.

Is using 2nd order elements a best practice when doing modal analysis with Optistruct?

Ben,

When using tetrahedral elements, first order elements are stiffer than 2nd order elements. That causes the numerical differences in the results, with results from 1st order elements showing higher modal frequencies, as you have seen in your initial run.

The 2nd order elements are recommended for static/modal analyses and would correlate much better to the results you would get from hexahedral elements or hand calc etc.