COMPARING RESULTS OF DEFLECTION IN CREO VS HYPERMESH

[schopra-2]

I have tried to do a chassis analysis in Creo Simulate using beam idealization and same in hypermesh but when I am comparing the results both show different value for the same loading scenario.can any one suggest why this of problem exist.

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.

[unickque]

This is impossible to answer without more information.

Tell us more about the way you modelled the chassis and the loading you applied?

[schopra-2]

CREO SETUP

I modelled the chassis wireframe and used beam idealization for assigning material and geometry of pipe to the wireframe in Creo and constrained all the four rear suspension pickup points in all 6DOF's.Then I applied vertically upwards force on Front right suspension points and downward force on front left suspension points and then I ran the analysis.

Same I did in hypermesh using same material properties .

If you have hyperworks 12.0 and creo 3.0 i can send you the files and you can look into it.

[unickque]

Yes if the files are not confidential please share them.

I'm on Creo2 and Hypermesh 13. Not sure if Creo2 will read v3 files, but i'll give it a try.

[schopra-2]

here are the links

Creo 3.0 .prt file (Dropbox - chassis.prt.1)

.igs file (Dropbox - chassis.igs)

hyperworks 13.0 file (Dropbox - sametube1.hm)

I dont have Creo 2.0.i have sent you .igs file maybe you can try to do the beam idealization with the .igs file in Creo Simulate.

[unickque]

Sorry, I can't get to Dropbox on my workplace

[schopra-2]

Then how can I share the files with you.Please do tell the alternative

[DenisJaunin]

Hello,

The tubular frame has always had many questions.

Sincerely.

Denis.

MCAD Central

Strengthening Automobile Chassis Using Finite Element Analysis - PdfSR.com

[schopra-2]

HERE ARE THE FILES

please do look into them looking forward for your replies

[unickque · Accepted solution]

Much better, thank you

Okay, so I can't read your Creo3 file since i'm still on Creo2 (unless someone can tell me how?) but I built the model from the igs file you gave me, using dimensions from the Hypermesh file.

My results:

HM12: max displ 1.157 mm

Creo2: max displ 1.175 mm

This is different than both of your results.

Some pitfalls that I can come up with:

* make sure to also constrain rotational degrees of freedom in Creo (default is only constrain displacements)

* make sure to check wheter your tube dimensions are correct (use radius, not diameter), I used outer radius 12.5 mm and inner radius 10.5mm because that is what was in the HM model.

* in HM make sure to turn on error checking; for some reason CBEAM 3050 and 3049 had a direction vector of 0,0,0 that i had to fix manually in the fem file before the model would run.

* check beam orientations; Creo2 for some reason still insists that you specify the orientation for a rotation symmetric beam profile, and does not use sane defaults when you select multiple lines

* watch out when applying forces; if you apply 100N on 2 points in Creo, it may be that Creo turns that into 50N per point (i'm not sure about this, I alway avoid this by modelling separate loads for each point)

* check units in Creo, use mmNs if possible

[schopra-2]

thanks patrick for your time .