I have imported a precise model from mechanical desktop to Patran and did a linear static analysis. In this analysis I used following units:
mm, kg, N, MPa

the material that I have used was stainless steel 304 with tensile strength about 250 MPa. But the result shows a stress tensor with maximum about 7000 MPa. In reality this part is working properly and there is no problem, so I concluded that a problem should be available in my modeling. Should I make any change in Units which I use? units like gravity or...

any comment or help?

It's important to make sure you use a consistent set of units.  NASTRAN is a "unitless" system and as long as you make sure your units are consistent, you shouldn't have problem.  Other things you might look at:

-Ensure that your boundary conditions and loading accurately model your part.

-Ensure that your peak stresses aren't a result of singularities caused by nodal loads or constraints.  If your peak stresses are near one of these, the stresses aren't realistic.  
    
-Check your displacements. If they're large, you might be outside the bounds of a linear static analysis and into the realm of geometric non-linearity.  If this is the case, try analyzing the model as a non-linear static model with large displacements turned on.  

-If you still have high stresses, you might need to add material non-linearity as well.  

I hope this helps.

DW

 

"On the human scale, the laws of Newtonian Physics are non-negotiable"

If you use mm; N; MPa You shall use Ton for mass. and Ton/mm^3 for densities.
As acceleration is mm/s^2, gravitation acceleration is 9810mm/s^2.

the force on a mass of 1kg shall be, in N, 9810* 1 * (0.001)=9.81 N
So to use consistent units mass shall be expressed in tons.
You could still use masses in kg, but remember to add to the solution PARAM    WTMASS .001
regards
Onda

Dear dwallace1971
Thanks for your response and help. I don't think displacements are too large so that the non linearity be appeared in the results.  

Anyway thanks for your kind response

Dear Onda

Thank you very much for your advise.

As I mentioned before I think this could be the major mistake that I have made. I try to correct it using your comment.
Could you please telling me how can I define the gravity value in Patran? Is it the Wt-Mass conversion in Solution parameters?

Looking forward to hearing from you

Gravity in nastran is set by the card ACCEL.
to apply gravity load in patran you should go under load>inertial load and set the correct direction and intensity. You do not have to select elements or grid points as the ACCEL will be for the entire model.
If you use, as I do, mm, kg, MPa, sec. the gravity shall be set in mm/sec^2 so the correct gravity will be 9810mm/sec^2.

As I use kg instead of ton, I need to add the PARAM WTMASS 0.001.
with this parameter, Nastran will scale all masses by the factor 0.001 and will transform all kg in tons. This is necessary to keep all units congruent, as I wrote before.
I prefer to use this parameter instead of write down masses in tons and densities in tons/mm^3 as this isn't very easy, numbers are way too small!

Dear Onda

Thank you very much
I applied your advice and it was really helpful.

About the contact analysis, if I want to have the contact forces, should I use MASTER/DBALL instead of XDB? and is there any other regulation which should be applied?

 

Master/Dball and XDB aren't comparable.
XDB is the file format to be attached to Patran.
Master/Dball are two files created by Nastran that you could use for a restart.

For contact you could use XDB and OP2 (I think so as I don't have the licence for contacts), the difference is that XDB is attached to patran while OP2 are loaded in patran, making the file heavier.
Onda