Is it possible to plot the reverse of the composite failure index in Hyperview?

Casper Kruger

Hi,

 

I am doing a benchmark simulation and require the reverse factor of the composite failure index. Is this output available in Hyperview or does it need to e calculated separately? 

 

Kind regards, 

 

Casper Kruger

Adriano Koga_20259

Are you looking for Strength Ratio?

 

The Strength Ratios that are output as a result of PARAM, SRCOMPS, YES depend on the Failure Theory specified by the user. The following equations show the relationship between the Failure Index and the Strength Ratio for different Failure Theories.

Hill Failure Theory:

StrengthRatio=1√FailureIndexStrength Ratio=1Failure Index

 

Hoffman Failure Theory: There is no direct relationship between the Strength Ratio and Failure Index (refer to Composite Laminates in the User Guide for more information). OptiStruct solves the quadratic equation to find the strength ratio.

Tsai-Wu Failure Theory: There is no direct relationship between the Strength Ratio and Failure Index. (refer to Composite Laminates in the User Guide for more information). OptiStruct solves the quadratic equation to find the strength ratio.

Maximum Stress (Strain) Failure Theory:

Strength Ratio=1Failure Index

 

Transverse Shear Failure Theory:

Strength Ratio=1Failure Index

 

If that's not exactly what your looking for, you can always create your own result from the Failure Index, by using Result Math,similarly to this thread here:

https://community.altair.com/community?id=community_question&sys_id=b3c8fb0fdb20a490e8863978f49619ad

Casper Kruger

Adriano

Thank you for the reply as well as the additional link, that will do the trick. Is there a way to run all the failure theories in one run and export the results to a table to compare? 

Adriano Koga_20259

Casper Kruger said:

Adriano

Thank you for the reply as well as the additional link, that will do the trick. Is there a way to run all the failure theories in one run and export the results to a table to compare? 

PARAM,ALLFT,YES or something like that. Not sure if this covers SR.

Michele Macchioni

Casper, 

you may want to check several failures as well outputting op2 results from OS and then use HV composite modules to run post cross evaluation.

We developed (motivated by Airbus request) an extra tool called "Composite Failure Wizards" which you can access from the Aerospace menu (OS profile) in HyperMesh.

You can use it to as well set the material allowables associated to the MAT8 cards.

The tool writes an XML statement which triggers then HV to process the data automatically without you having to input the expression in derived results. 

I have attached a quick video for the same.

Extra tip: if you run HVTRANS on that XML you get as well the h3d version of it.

Hope this can help you further.

Regards

Michele

Casper Kruger

Michelle, 

 

Thank you for the video, it does help thank you. Just so the thread is complete, I received the below method from customer support as well:

1. You can export a set of results by using the aerospace tools in Hypermesh.
2. If you import your model in HM and change the user profile to Engineering solution -> aerospace, aerospace tool will become available
3. From there click on File Loader to load the results file and import it.
4. Then click on results query
5. And select the results you want to save in a csv file

 or

1. Try with the build plot tool in HV to reduce the number of clicks.
2. Here you can select your set of results (stress, strain, failure index) and plot all the relative results in a graph.
3. If you click on the plot, the export curve button will become available and you can export all the data to a csv file

Thank you,

 

Casper Kruger

 

 

 

Michele Macchioni

Casper Kruger said:

Michelle, 

 

Thank you for the video, it does help thank you. Just so the thread is complete, I received the below method from customer support as well:

1. You can export a set of results by using the aerospace tools in Hypermesh.
2. If you import your model in HM and change the user profile to Engineering solution -> aerospace, aerospace tool will become available
3. From there click on File Loader to load the results file and import it.
4. Then click on results query
5. And select the results you want to save in a csv file

 or

1. Try with the build plot tool in HV to reduce the number of clicks.
2. Here you can select your set of results (stress, strain, failure index) and plot all the relative results in a graph.
3. If you click on the plot, the export curve button will become available and you can export all the data to a csv file

Thank you,

 

Casper Kruger

 

 

 

Hi Casper,

the above workflow support provided to you are correct when it comes to output multiple available data into a CSV and they work pretty slick. 

I am personally bound to the Results Query tools as I had been overseeing its development

That being said, the workflow I passed you is indeed aimed to:

- create new results (several composite failures in one shot)

- control/change (if required) material allowables (so you can trade-off several variants)

Surely, once the h3d is for instance available you use any of the mentioned tools to export such data.

More is as well to come as we are working to directly connect Matrix Browser with results entities in NGHW.

Thanks and regards

Michele