Adding a spring to the model

Hi,

You can run a solid spring with a contact pair by compressing it until the correct position. After exporting the deformed mesh and using ASSIGN with the .h3d generated from this analysis to your sandwich assembly and resolve the initial stress with INISTRS.
Unfortunately, map strain is still under development. However, initial stress should work for you.
Please take a look at the files and let me know if work for you.
The example attached uses a text file for the stresses, however, you can use the .h3d file instead.
Also, mark the answer as correct if solves your question. This will help others.

PS: If you desire to compress the spring while applying the pretension load you can just use a spring solid mesh and apply the bolt pretension directly. It would not be necessary to use initial stress. For both cases, you need to use NLSTAT (nonlinear solution with LGDISP) considering the contacts.

Thank you very much,

Hi,

You can run a solid spring with a contact pair by compressing it until the correct position. After exporting the deformed mesh and using ASSIGN with the .h3d generated from this analysis to your sandwich assembly and resolve the initial stress with INISTRS.
Unfortunately, map strain is still under development. However, initial stress should work for you.
Please take a look at the files and let me know if work for you.
The example attached uses a text file for the stresses, however, you can use the .h3d file instead.
Also, mark the answer as correct if solves your question. This will help others.

PS: If you desire to compress the spring while applying the pretension load you can just use a spring solid mesh and apply the bolt pretension directly. It would not be necessary to use initial stress. For both cases, you need to use NLSTAT (nonlinear solution with LGDISP) considering the contacts.

Thank you very much,

Hi @Robinson Ferrari , 

Firstly, thanks for the detailed explanation.

I want to compress the spring as you stated. But, when I add the spring to the model as in its original position, I have a convergence problem because of the gap between the components.

1. So it made sense to me to compress it down to the compressed position and add pre-stress. Thank you. If I add a thermal load step to this model, will it work?
2. How to export stresses in 2 components from a submodel consisting of 4-5 components (spring deformed)?

Thank you. 

Best Regards, 

Ovunc

Hi @Robinson Ferrari , 

Firstly, thanks for the detailed explanation.

I want to compress the spring as you stated. But, when I add the spring to the model as in its original position, I have a convergence problem because of the gap between the components.

1. So it made sense to me to compress it down to the compressed position and add pre-stress. Thank you. If I add a thermal load step to this model, will it work?
2. How to export stresses in 2 components from a submodel consisting of 4-5 components (spring deformed)?

Thank you. 

Best Regards, 

Ovunc

Hi Ovunc,

1- Yes, it should work
2- You can export the deformed mesh using HV, and then use the .h3d generated by your simulation in the new model (with exported geometry) and use ASSIGN mentioning the set ID (ESETID#) you want to apply the initial stress. In our documentation there is all information you need for this.
INISTRS should be like this:

$
ASSIGN,H3DRES,100, 'OneStep.h3d'

$$
SUBCASE 1
LABEL Default
SUBTITLE = Default
ANALYSIS NLSTAT
SPC = 1
NLPARM = 1
INISTRS = 4
$
INISTRS 4 100 1
+ ESET 2
Thank you very much

Hello, 

Thank you for support. I have some questions. I would be happy if you evaluate the following items separately.

1. I used to deformed mesh, .h3d file and ASSING. But, I cannot select the h3d file in the ASSING command. In my model, the name of the h3d file can only be written by hand. So file location etc. cannot be selected. So, the h3d file cannot be found.
2. I used to deformed mesh, Bulk_Unsupport_Card and Initial stress.blk file. How can I create the .blk file for a different scenario?
3. I want to not use the first two items, but to solve different load steps in a single .hm file. In other words, the spring is compressed using non-linear static or linear static analysis in load step 1, and the bolt is torqued using non-linear static analysis in load step 2. So, can linear analysis be added as a subcase to the pretension analysis?

Thank you. 

Best Regards, 

Ovunc

Hello, 

Thank you for support. I have some questions. I would be happy if you evaluate the following items separately.

1. I used to deformed mesh, .h3d file and ASSING. But, I cannot select the h3d file in the ASSING command. In my model, the name of the h3d file can only be written by hand. So file location etc. cannot be selected. So, the h3d file cannot be found.
2. I used to deformed mesh, Bulk_Unsupport_Card and Initial stress.blk file. How can I create the .blk file for a different scenario?
3. I want to not use the first two items, but to solve different load steps in a single .hm file. In other words, the spring is compressed using non-linear static or linear static analysis in load step 1, and the bolt is torqued using non-linear static analysis in load step 2. So, can linear analysis be added as a subcase to the pretension analysis?

 

Thank you. 

Best Regards, 

Ovunc

Hello @Robinson Ferrari, 

Do you have any advice on topic?

Thank you so much. 

Best Regards, 

Ovunc

Hello @Robinson Ferrari, 

Do you have any advice on topic?

Thank you so much. 

 

Best Regards, 

Ovunc

Hi Ovunc,

I'm sorry for the delay, I was on vacation.

1 - Please take a look at the file attached as an example. You don't need to inform the path, just keep the .h3d file in the same folder.

2 - The .blk file was used only as an example. It's a text file, in your case you will use the .h3d file.

3 - For using CNTNLSUB you need to use nonlinear even for load step 1. However, you can define the continuation from load step 1 for the other subcases (for example, subcase continuing from subcase 1 and subcase 3 continuing from subcase 1 as well).

Please, take a look at this session from our documentation for INISTRS: https://2022.help.altair.com/2022/hwsolvers/os/topics/solvers/os/inistrs_bulk_r.htm?zoom_highlight=INISTRS

I would like to recommend our OptiStruct Non-Linear training, it's free. You will have access to all OptiStruct non-linear capabilities, including INISTRS, CNTNLSUB, and so on.

Thank you very much,