How to define Inertia Relief Analysis
Altair EmployeeHello,
Inertia Relief analysis is the analysis of unconstrained structure e.g. a plane in flight. The applied loads are balanced by a set of translational and rotational accelerations (automatically determined by the solver) instead of reaction forces (as with 'classic' boundary conditions).
To define inertia relief, please define SUPORT instead of SPC in the constraints menu. The degrees of freedom are the same as with SPCs. You can also define param inrel -2 in the control card section to automatically determine accelerations on the model for force balance.
A description of inertia relief can be found in the help:
<PATH>/hw13/help/hwsolvers/hwsolvers.htm?loads_and_boundary_conditions.htm
or in the Basic OptiStruct tutorials
OS-1030: 3D Inertia Relief Analysis using OptiStruct
Best Regards
Jan
Answers
-
Hello,
I was just trying to setup a small model to test the Inertia Relief function and I'm having a little trouble to get the analysis going.
The front left point shall experience a bump of 500 N while the other three corners are constrained, e. g. like a car on a street driving over a road bump.
The DOFs of the constraints are defined like this:
- back/right constraint: 12346 are fixed (SUPORT1).
- back/left constraint: 12346 are fixed (SUPORT1).
- front/right constraint: 234 are fixed (SUPORT1).
<?xml version="1.0" encoding="UTF-8"?>
(see attached Picture_1.jpg)
The PARAM-INREL is set to -1.
When I'm trying to start the analysis, I get the Error #798:
'The maximum number of support d.o.f. is six.
SUPORT1 set id = 13
number of support d.o.f. = 0'
I've already tried the following things:
- changed the load type of the constraints to SUPORT:
--> Result: Error #23: 'SID 2 used on Case Control data SUPORT1 is missing in bulk data.'
- deleted PARAM-card:
--> Result: Analysis finishes, but there is no difference between the analysis with Inertia Relief and the analysis without Inertia Relief.
- changed the number of DOFs to:
back/right constraint: 123 are fixed (SUPORT1).
back/left constraint: 13 are fixed (SUPORT1).
front/right constraint: 3 are fixed (SUPORT1).
--> Result: Analysis finishes, but results differ widely from expected result and also the result without Inertia Relief.
<?xml version="1.0" encoding="UTF-8"?>
<?xml version="1.0" encoding="UTF-8"?>
(see attached Picture_2.jpg and Picture_3.jpg)
Normally, the results should not vary that widely from each other, do they?
So my question is now: how do I set up the constraints correctly to make the analysis work?
Thanks a lot in advance!
Dominik
0 -
Hi Geusken
I think the second approach you had made is correct.
the forces are calculated that results from a rigid body acceleration of the SUPPORT1 degrees of freedom in the specified directions, provided Up to six degrees of freedom can be defined per sub case.
0 -
Hi Prakash,
I think I found my mistake.
I used a shell thickness that was way too thin (1 mm), so the whole body wasn't stiff enough against torsion and each flat surface deformed for itself. (See the aforementioned Picture_2.jpg of the last approach)
Since this is just an experimental model to see the effects of the Inertia Relief analysis, I set the thickness to 5 mm to stiffen the whole body against torsion and now the results seem to make more sense.
Thanks for your help!
Dominik
0 -
Hi guys,
how can I output or check the interia relief values of my calculation? Is it an output file or do I have to define specific output for the result file?
0 -
Hi,
I really need some help with my inertie relief analysis.
How is the REFERENCE POINT which is given in the output for inertia relief calculated? I expected it to be at the center of gravity but that is not the case. Is there an option to change the reference point and set it to the center of gravity or to any desired node of the mesh? My resulting inertia relief accelerations differ from the self-calculated values...but I have calculated them around the center of gravity, but in Optistruct my reference point is another one...
I tried to add PARAM,GRDPNT option but it does not work and to be honest I am not sure what I am doing.
0 -
Altair Forum User said:
Hi,
I really need some help with my inertie relief analysis.
How is the REFERENCE POINT which is given in the output for inertia relief calculated? I expected it to be at the center of gravity but that is not the case. Is there an option to change the reference point and set it to the center of gravity or to any desired node of the mesh? My resulting inertia relief accelerations differ from the self-calculated values...but I have calculated them around the center of gravity, but in Optistruct my reference point is another one...
I tried to add PARAM,GRDPNT option but it does not work and to be honest I am not sure what I am doing.
Hi, can anyone help me on this topic?
0 -
Altair Forum User said:
Hi,
I really need some help with my inertie relief analysis.
How is the REFERENCE POINT which is given in the output for inertia relief calculated? I expected it to be at the center of gravity but that is not the case. Is there an option to change the reference point and set it to the center of gravity or to any desired node of the mesh? My resulting inertia relief accelerations differ from the self-calculated values...but I have calculated them around the center of gravity, but in Optistruct my reference point is another one...
I tried to add PARAM,GRDPNT option but it does not work and to be honest I am not sure what I am doing.
Hi there, I would like to repeat this question:
I have examined already 3 different models and the automatically calculated reference point NEVER matches the center of gravity of the structure. That is why the resulting accelerations differ from what I expect from manual calculations.
Can you please tell me how OptiStruct calculates the reference point and how to make the solver set the center of gravity as reference point?
0 -
In inertia relief, the reference center is not COG but the average of the coordinates of all the grids in the model.
The x-ref to be sum of all x-coordinates of the all the grids divided by the number of grids in the model. Similarly for y-ref and z-ref.
This will match the COG when there is a uniform mesh and not if the mesh is random.
am checking if there is any way to change the reference point to the COG
0 -
Hi,
Ref point can be changed using the PARAM,REFPNT card
0 -
0
