Good afternoon everyone, I've just upgraded to v11.1 from 10.3 and I've been happy to discover you can now use bolt preload on solid elements. Only thing is now, how do I use it? Anyone know of any good guides or anything? I have managed to do it, but not really sure I'm doing it right. For example what is Ref plane node for? and is it best to select all elements of a bolt or just some in the middle?
Any help and guidance would be much appreciated.
Solved! Go to Solution.
To define the solid bolt, only select a "slice" of the bolt, either by grid or elements. See the NX Nastran 8.5 Release Guide Chapter 10 where this capability was added to Nastran for a description of what happens inside Nastran. I think this will help you understand the inputs that you are selecting in Femap.
Just got back round to this when I needed to use it. Many thanks for the pointer, I'd only been looking in the FEMAP documentation, didn't think to look in the nastran files.
One point though, it doesn't say anything about selecting only a slice, in fact it seems to say to select all elements of the bolt. I was just wondering why you said to select only a slice?
From the Nastran User's Guide:
Modeling with Solid Elements
The structure of an input file for modeling bolts with solid elements is identical to that for modeling bolts with line elements except that:
• A mesh of CHEXA, CPENTA, and CTETRA elements are used to represent a bolt. Create the solid element mesh such that at an intermediate position along the bolt axis the element edges and element faces of the mesh form a cross section through the bolt. As a best practice, make the cross section planar and normal to the axis of the bolt. Doing so will facilitate interpretation of the results. The cross section of the mesh and the material properties associated with the mesh should also be representative of the corresponding bolt.
I've attached a sample model that uses a General Solid body (Non-manifold solid) that has a plane cut at the location of the interface between the two lugs for the location of the Solid Bolt Pre-load. Note that there is also a Coordinate System that is used to define the direction of the pre-load. The nodes used for a pre-load must be coincident.
I hope this helps.
Principal Femap Applications Engineer
I have been struggling for some time with the preload setup on the solid bolt.
I followed most of the guidelines you stipulated, the error I receive is as follows "No CHEXA, CPENTA, and CTETRA grid forms part of bolt #". This is very strange as I can see the selected grids under the bolt region. I have modelled the bolt with tet10 elements.
What to do with the direction of the preload when the orientation of the bolt with respect to the global coordinate system is off-set?
I have revised the posted FEMAP model using FEMAP V11.2.1 and ran the LINEAR STATIC CONTACT analysis (SOL101) and in fact, I receive the following error message:
M O D E L S U M M A R Y NUMBER OF GRID POINTS = 80322 NUMBER OF CTETRA ELEMENTS = 52086 *** USER FATAL MESSAGE 22201 (MODGM2BC) BOLT GRID 2028509 IS NOT CONNECTED TO ANY ELEMENT THAT LIES ABOVE
THE DEFINED CUT PLANE. THIS COULD BE DUE TO SKEWED ELEMENT SHAPES OR
IMPROPER DEFINITION OF BOLT DIRECTION.
Revising the BOLT PRELOAD REGION definition I see the reason of the error, the axis selected to orient the bolt region is wrong!!. The one selected is the local X axis using CS#101, but in the picture this is not the longitudinal bolt axis, the correct one is the local Z axis.
In fact, after selecting Z-axis as BOLT AXIS, then the analysis runs OK, here you are the result. Please note I STRONGLY suggest always to mesh with solid CHEXA elements instead of TET10 elements because with bolt preload + contact the Element Iterative solver is not supported yet using NX NASTRAN 10.1, you will get the following error:
*** USER FATAL MESSAGE 22201 (MODGM2B) ELEMENT ITERATIVE SOLVER CANNOT BE USED IN A PRELOADED
BOLT ANALYSIS WITH BOLTS COMPOSED OF SOLID ELEMENTS WHEN CONTACT IS PRESENT * * * END OF JOB * * *
Then in order to reduce the solution time (and increase accuracy of the result!!) better try to mesh with HEXAEDRAL elements CHEXA instead TETRAEDRAL elements CTETRA:
thank you so much with the responses, I'm satisfied.
On my latter question about the bolt orientation being off-set from the global coordinate system, how does one setup "Local bolt axis using CS#10"?
The bolt axis not need to be coincident with the global coordinate system, you simply need to select any of the global axis that is parallel with the bolt axis.
In the case that your bolt axis is not coincident neither parallel to the global coordinate system axis, then simply create a LOCAL COORDINATE SYSTEM (in this example is the 101) using the command MODEL > COORDINATE SYSTEM with the multiple methods you have (by angles or by workplane) and use the correct axis of this local coordinate system to define the BOLT PRELOAD REGION.
Remember: the global or local axis should be aligned with the bolt-axis, OK?.
If I may add something to this conversation.
I tried with a good result, to apply the bolt preload via temperature load. Lowering the temperature causes the element shrinkage and therefore internal forces in bolt.
It is just a matter of proper scaling of the temperature load that we want to apply.