Find more posts tagged with
- I have 3 excitation points.
- Each of the excitation points have an RLOAD1 definition in x, y and z.
- Giving a total of 9 excitation profiles which I have defined via the load collectors.
Hi @IRA_EM
Please take a look at the attached tutorial in the documentation.
The only difference it that you're going to replace the DAREA for a SPCD (enforced displacement), and in the same node, you will create a SPC at the same DOF as the SPCD.
So, for example, for enforcing Y displacement in node 1000, you create a SPCD in DOF2, with value 1.0 for, and in the SPC load collector, you create a SPC = 0 in DOF 2, as well.
@IRA_EM In addition to Adriano's answer, I think you will also need to specify Type as 'DISP' in RLOAD2 card for enforced displacement
Hi Adriano and Nathan,
Thanks for the tips. I now have the following problem.
The problem I have is how to combine these for assignment to the DLOAD entry in the subcase definition of Freq.resp (modal).
I thought I could combine the RLOAD1s into 1 load collector but therein lies the problem, as only one EXCITEID can be selected where in fact there are 3....
Any ideas are welcome
you will have 9 RLOAD cards, each one pointing to its own EXCITEID and TABLED1.
For X_point1, you will have a RLOAD1 pointing to the SPCD in X for point 1.
For Y_point1, you will have a RLOAD1 pointing to the SPCD in Y for point 1.
and so on..
in the end the DLOAD load collector will combine all you RLOAD1 cards into a single one, applying them all together.
This will be refereced in your LoadStep.
Don't forget to constraint with regular SPC each point and DOF where you apply the SPCDs.
Do you have an error or something? Can you share the .out file?
This is a shaker, right?
Can you describe better your test input and desired output?
do you want to experimental data ?
I would like to reduce file size of the model for example I would like to avoid solid elements
I would like to reduce run time?
i'm trying to understand better, physically, what are you trying to simulate here.
Can you describe better what are your test inputs, and desired responses?
First of all>
You're running Direct Frequency Response, which is very expensive computationally, as you're solving the equations coupled.
Usually we would use Modal Frequency Response for such problems. (Tutorials in OptiStruct help section)
I believe that your honeycomb modelling is ok, using shell elements.
The plate from the test jig doesn't need to ne solid, nor so refined.
You could use a simple shell model, and use some freeze contact (TIE) to keep the plate tied/glued to your honeycomb.
The plate would be the master, and your honeycomb the slaves.
There are a few tutorials in OptiStruct help, for contacts, if you're not familiar to it.
Another point is the output size.
You're requesting FREQ1 with 1Hz increment.
So all your results will be written for several frequencies, increasing memory requirements.
I would suggest you to take a look at FREQ4 (oly for Modal FRF). It takes a few points close to the natural frequencies of your model.
You could mix FREQ1 by 10Hz, and FREQ4 including 3 or 5 points.
Actually it depends a little bit on your frequencies. I believe in your model there are a lot of modes close, so maybe increasing the number of frequency points only close to these points.
Also for larger models (~1M nodes) using EIGRA instead of EIGRL it is a good approach. EIGRA uses AMSES solver, which applies sub-structuring for enhancing a lot the eigenvalue extraction, while introducing a small 'simplification'.
Speaking on eigenvalues, you're requesting only 15 first modes.
I'm not sure if this is enough for performing your analysis if you use Modal FRF.
Usually in these cases the rule of thumb is at least 1.5x the frequency of interest. So if you're interested in frequencies up to 200,Hz request EIGRL/EIGRA up to 300Hz. This is related to modal space for your solution.
https://community.altair.com/community?id=community_question&sys_id=524600b61b2bd0908017dc61ec4bcb67
.
i'm trying to understand better, physically, what are you trying to simulate here.
Can you describe better what are your test inputs, and desired responses?
First of all>
You're running Direct Frequency Response, which is very expensive computationally, as you're solving the equations coupled.
Usually we would use Modal Frequency Response for such problems. (Tutorials in OptiStruct help section)
I believe that your honeycomb modelling is ok, using shell elements.
The plate from the test jig doesn't need to ne solid, nor so refined.
You could use a simple shell model, and use some freeze contact (TIE) to keep the plate tied/glued to your honeycomb.
The plate would be the master, and your honeycomb the slaves.
There are a few tutorials in OptiStruct help, for contacts, if you're not familiar to it.
Another point is the output size.
You're requesting FREQ1 with 1Hz increment.
So all your results will be written for several frequencies, increasing memory requirements.
I would suggest you to take a look at FREQ4 (oly for Modal FRF). It takes a few points close to the natural frequencies of your model.
You could mix FREQ1 by 10Hz, and FREQ4 including 3 or 5 points.
Actually it depends a little bit on your frequencies. I believe in your model there are a lot of modes close, so maybe increasing the number of frequency points only close to these points.
Also for larger models (~1M nodes) using EIGRA instead of EIGRL it is a good approach. EIGRA uses AMSES solver, which applies sub-structuring for enhancing a lot the eigenvalue extraction, while introducing a small 'simplification'.
Speaking on eigenvalues, you're requesting only 15 first modes.
I'm not sure if this is enough for performing your analysis if you use Modal FRF.
Usually in these cases the rule of thumb is at least 1.5x the frequency of interest. So if you're interested in frequencies up to 200,Hz request EIGRL/EIGRA up to 300Hz. This is related to modal space for your solution.
https://community.altair.com/community?id=community_question&sys_id=524600b61b2bd0908017dc61ec4bcb67
.
I aim compare vibration isolation characteristic of the honeycomb specimen
so I preferred to calculate direct FRF, also @Rahul R suggested me that direct FRF is more availeble
I have a model in attachment
but this model do not agreed wit experimental data
i believe the forum is the best way to solve any question, and additionally the solution of your problem might be useful for others.
it would be nice for you to share here what are the differences that you found between FEA and tests.
1) normal modes are ok?
2) mass is ok?
3) what is the shaker input?
4) what are you measuring? acceleration? displacement?
in the model I shared first, four of mode frequencies were agreed with experimental results but experimantal test rig is not enough to determine mod shapes and I have not enough accelerometer
mass of real rigid plate and mass in numerical model are agreed
shaker input is acceration of .25 g
output is acceraiton
also impact hammer test was performed on this concrete
the honeycomb specimen with rigid plate was glued to the metal plate, which embedded to concrete using adhesive .
the results from this experiments were agreed to numerical results
yes some frequencies of fem model were agreed with experimental results from this test system
in this test honeycomb specimen with rigid mass was bonded using an adhesive material and tests were performed with impact hammer
I assumed that bottom of the honeycomb is clamped I'm not sure if this is true or not.
Hi @IRA_EM
Please take a look at the attached tutorial in the documentation.
The only difference it that you're going to replace the DAREA for a SPCD (enforced displacement), and in the same node, you will create a SPC at the same DOF as the SPCD.
So, for example, for enforcing Y displacement in node 1000, you create a SPCD in DOF2, with value 1.0 for, and in the SPC load collector, you create a SPC = 0 in DOF 2, as well.
Unable to find an attachment - read this blog