Displaying End A/B Results in Patran

[Stezza]

Hi,

I want to display in Patran, as a vector, the bending moment of a bar element at End A and End B. Is this possible as I can't seeem to find the option in the results "tab"?.

I know that the results exists, as I can see the bar element results for bending moment at end A and end B in my .f06. Thus from the .f06 I know what the results are but I want a screen shot for a report and a vector would be helpful to show the sign convention/axis orientation.

If you know how to get these results graphically on the screen some directions would be appreciated.

Details are MSC.Supermodel 2005r2
Output request used ELFORCE = ALL
.OP2 file used

Thanks
Stezza

 

[Onda]

I think you should change the additional display control on second tab of result - create - marker - vector
and set the additional display control to nodes

See pictures for clarification.

Onda

 

[gokmavi]

Stezza,

As far as I know (I could be wrong), it is not possible with PATRAN what you want to do. It either shows average values at the center of the element or values at the nodes at two ends but again by averaging with values belonging to the common node of adjacent element. It does not present results as inf06 file i.e. it does not show end A & end B moments for each individual element. If somebody knows a way doing it please let us know.
Onda, solution what you proposed is not what Stezza wants.
Regards.

gökmavi

 

[Stezza]

Hi thanks for both the replies.

Onda - when I try additional display control nodes I don't get the bending moment I expect from the results in the .f06 file - I suspect that as gokmavi said it is the average of the surrounding nodes.

Thanks

 

[Onda]

Bending moment @grid X respect to element Y and respect to element Y+1 MUST be the same except if is a T joint.
I don't think is an averaging problem!
Just open the f06, and check it!

Maybe you should disply bending moment by components? on the F06 you have components (in beam coordinate system). On patran you must ask to disply by components (in as IS coordinate option). Default is resultants.
Try to do a very easy model, (a bar with one fixed end and one force) and compare patran to f06 results.
Then try to modify plane of force and property of sections in way to understand when you get the difference.
On my model, i get exactly the same bending moment on F06 and patran.

As last possibility just post on the screen one element with the two grids.
Ask to Average to Target entity, then Patran should not average (target is only one element) and disply only the bending moment on that element @grid X and grid X+1.

Onda

 

[gokmavi]

Dear Onda,
It seems that Stezza's model is not a simply loaded simple beam model. Assume he has a skin stringer model or bar elements he mentioned are caps of a typical spar structure. In this case, bending moments at the same grid but belonging to the two adjacent elements would not be the same.
Regards.

gokmavi

 

[Onda]

I've done a simple beams model with grids shared with shells elements.
The first model is made with 20 Cquad4 and 10 Cbeam and I noticed in the F06 a difference in the Bending Moment Result between grid X and Grid X+1.
Then I've doubled the number of beam and quadrupled the number of cquad and the difference become smaller.
Then I've refined the model again and the difference become even smaller.

The Bending moment shown by Patran is the average of the two Value read in the F06 and is the converged value of the model.

I don't know why on the F06 there is a difference between Bending moment of beam Y at grid X and Beam Y+1 at same grid point but, for a mesh converged model, this difference become close to 0.

Attached there is a print screen of four models and the convergence graph.

 

[Stezza]

It's interesting to see the details of how the mesh effects the patran results.

For me I do have multiple parts comming together at one location. Lateral floor beam (bar-quad-bar), longtidunal steat track (beam). Floor Panels (quads). Also the mesh is very coarse - global FEM model.

The simple solution I went with was just use the f06 results.

Thanks for the input.