I've been tasked withdoing an analysis (random response) to help my company select isolators to use for a product we are building. I am very new to FEMAP (as in just learned it existed when assigned this) and have only used a little ANSYS for static analysis in school as far as FEA goes. From searching around, it seems like the best way to model springs, by large consensus, is CBUSH elements. However, each time I've used them, I get SEKRRS errors. They sometimes say the issue is in rotational DOF's and sometimes in translational DOF's.
The resources I find online have explained that CBUSH has 6 DOF while solids have 3. So, they say to constrain the ends in rotation, or add a high rotational stiffness. However, that has yet to solve any issues. I'm sure that this shouldn't be hard, and that I'm missing something. I found a slideshow here that showed CBUSHes between non-coincident nodes and attached to a solid, but I haven't been able to replicate it. I attached a really basic mass/spring/damper that I made which shows the error. My long-term goals for this would be 4 elements near the corners of a rectangular solid on the bottom face. They each would have vertical and horizontal stiffnesses and then I could inject PSD's into the node at the base of them. Also, I will want to do these between two solids which I would guess have to be offset so contact isn't simulated. All of this is for vibration and shock isolation. However, to start with, I'd just like help understanding where I'm going wrong.
Before I forget, I've used the grounded CBUSH macro that comes in FEMAP. That works just fine. Since I need isolation between solids, that probably won't work though. I also want to be certain that, when injecting a PSD, I am putting it into the base of the isolator, not the node that is on the part. Thanks for any help!
Solved! Go to Solution.
If you plan to run a Random dynamic analysis you first need to be able to solve the basic problems, start with linear static and modal eigenvalue analysis, you need to know the behaviour of the NX NASTRAN FINITE ELEMENT LIBRARY (in FEMAP click in HELP > NX NASTRAN, take a look to the USER's GUIDE, etc..).
In this problem you have different rigid body motions, this is the main reason of the error, your CBUSH don't have stiffness in the X & Y directions. You need to stabilize the CUBE elements. It´s more: not matter if you enter non-zero stiffness values in the ALL 6 DOF, you will continue having rigid body motions because your CBUSH is a point (you are constraining the movement of the CUBE in the Z-axis, not with infinite stiffness, but with k=100), you need to constraint also the X & Y movements.
To understand the free body motions in your model simply run a normal modes/eigenvalue analysis using NX NASTRAN (SOL103), you will see the following rigid body motions (please note how mode#1 to mode#5 has values of zero Hz, ie, rigid body motions):
Only MODE#6 has a value different to 0 Hz, this is a "genuine" rigid body motion in the Z-direction, the whole CUBE move rigidly in the direction of the CBUSH axial stiffness:
In summary, you need to remove the rigid body motions of the cube, either using nodal constraints (restricctions) or using another springs, ie, CBUSH elements. Here you are an example, but it depends of the real problem needs: as you see the first MODE#1 has a value of f1=20.78 Hz, then if you run a LINEAR STATIC ANALYSIS with NX NASTRAN (SOL101) you will have an answer, not erro, OK?.
Well, this reply is awesome. I followed it and did both things you suggested. I applied T1 and T2 constraints on the solid, which worked. Then, I tried putting 4 CBUSH elements on the base. With both of those methods giving me 10 non-zero modes (as you can see in the picture below), I did some static loads (both vertical and horizontal) and things looked good.
I then followed this up with a random response by injecting a PSD first in only vertical, then in all 3 axes to a rigid element connecting the 4 elements. The spikes in the output accelerations matches up really well with the modes I found earlier and made sense.
Now, I'm trying to move onto a 2-body model, because the final system I want to create will probably be something like that. I started with the modal analysis like you suggested and found 3 modes at 0, which means I have unconstrained motion. When I animated them, all 3 affected the top block only. That says to me the the unconstrained motion is in that block. Now, I want to figure out how to constrain this motion appropriately. I'm interested in the output acceleration in all 3 axes on it, so, I don't want to constrain the block, I think. I'm going to try running a static analysis and I think that will tell me what constraints are needed. I've attached the model so you can see where I got so far.
Thanks for all the help, I've been banging my head against a wall for about 2 weeks trying to figure this out.
For a general guide on solving singularity 9137 errors, there is one here:
With this model, your problem is that the stiffness of your CBUSH elements cannot be properly utilised because the solid element nodes have no stiffness in rotation. Below is a suggested workaround for this problem using rigid elements to connect the CBUSHes over a small area (I have shown 3 alternative patterns, but the principle is the same). In this case, the translational stiffness at the "leg" nodes of the rigid element now support rotational stiffness at the centre node where the CBUSH is connected. Thus the stiffness values on your CBUSH elements will be used. And if you are designing isolation mounts, your real structure is not going to have these forces/moments transferred through points of "zero area" - it is realistic to spread the transferred load over an area.