As I wrote, in our office we have Basic Bundle of the NX Nastran, so the solver 106/601 is not available. I tried to perform analysis with simplified contact including material nonlinearity and I am wondering, whether it is possible to do. Of course the friction is not a case in here.
I tried two ways:
- model contact between to objects by use of CBUSH elemetns, which have infinite stiffness in compressin and zero-stiffness in tension. I connected bodies surfaces by using 1D connection (nodes-nodes), however there was some issue with defining coordinates for the CBush elements?:
WARNING Some "CBUSH" elements in mesh "bush_springs:connection_mesh(2)" do not have an orientation specified. ACTION: Define an orientation for the mesh in the "Edit Mesh Associated Data" dialog or define an orientation for each of the elements using Element Associated Data.
I switched it to CSYS overriding and in final it looks, that the stiffness of the springs was not taken into account. Model just flew away.
The idea was to do something similar to techinque presented on this movie: femap - non linear constraint
- second idea was to use glue option. Is there a way of putting parameters defining "strength of the glue", so it will not "act" or the glue will crash under certain tension forces ?
Do you have any experience you would like to share with such kind of analysis ?
thanks for help
Yes I know that, but I just wanted to do some "research" of other techniques and to take the material non-linearity into account.
I just tried to follow the tutorial from link and it seems to not work for me. Could anyone see the attached fem & sim file and say what is wrong with this model ?
It seems that the cBush spring does not work properly. Ramp function is specified but it looks that the stiffness of the spring is not taken into account :/
To solve contact problems using the basic nonlinear module (SOL106) not need to use CBUSH elements, you can use perfectly 1-D node-to-node CGAP elements where you can set tailored to be compression-only elements, I remember writting a post regarding how to mesh with CGAP elements in NX AdvSim V10:
Only in the case where you need to define a nonlinear relation between force vs. length (ie, nonlinear stiffness) then you can use a CBUSH element and solve the problem as nonlinear.
Thank you Blas,
It's CGAP is something new for me I will try to test it in practise. But when it comes to the model i putted above (bush.zip). I meet still a problem with this model. It does not work and I have no idea why. All the properties are specified correctly (I suppose).
Could you please tell me why this is not working ?
End of topic. I managed to do solve this problem with use od CGap and Cbush elements as well.
What could be a tip for others, as I can see in FEMAP, user do not need to specify the orientation vector for Cbush (and probably for Cgap elements too, I do not have Femap but I can assume so). What was misleading me, the orientation vector user need to provide in NX environment is a Y (?) local vector of the connecting element. This was tricky and by mistake I overwritten local connector X-axis with global X-axis. This caused not including of the spring stiffness.
And now new question appeared. I wanted to generate animated gif of my screen with many viewports (as on screenshot). When play an animation, everytking is ok, all the viewports are sychronized but when I export a gif, only one viewport is beeing exported. Is it possible to export them synchronized all together ?
If I open your nastran model in FEMAP I see the orientation of the PBUSH property is missing (a common error, by the way). And yes, in FEMAP you need to define the orientation of both CBUSH and CGAP elements as well, of course!. In NX AdvSim use command "Edit Mesh Associated Data" to orient correctly the CBUSH element.
When you define your study activate the option to treat CGAP elements as linear contact, not spring:
your CBUSH is defined nominal with 1N/mm in X-direction but your global CS points in Z-direction. May be thats why you don't get the right results. Its only a guess but perhaps its a kind of global scaling factor?
May be you only see beam bending results because your beam is fixed in all 6 DOFs. Try to free the rotation DOF Y-axis and see what happens. If your CBUSH in Z-direction works, your system should be well defined. But if not, you should get huge deformation in Z and rotation around Y.
Additionally, compare your analysis results with beam bending analysis without CBUSH element.
May be it helps.