Learning Forum

[kaiyeungli]

Hi there,

I am conducting structural analyses on ANSYS Workbench where I often have stress singularities in the corners.

I am not interested in those areas and want to hide those elements, and re-plot the stress contours with the correct range (i.e. one which ignores the fictitious maximums from singularities) .

Does anyone know how to do this?

I only post I found regarding this was from here, which I didn't find very helpful.

Kind regards,

Kai-Yeung

 

[sathya]

Hi,

Use worksheet and named selection to create group of desired elements.

[kaiyeungli]

Is it possible to hide just the elements within a named selection when visualizing the results? I only see the option to 'Hide bodies in group', which hides the entire body/bodies the elements are located in. I only want to hide 1-3 elements, where there are singularities.

[sathya]

Hi,

Create named selection of elements ignoring the ones @ singularity region.

In stress choose scoping method to Named selection and evaluate the result.

[kaiyeungli]

I see, so you have have create a Named Selection by: Mesh Element - Element ID - Not Equal - 'element no. I want to exclude'.

Thanks Sathya.

 

[andimens13]

Please I am having the exact same problem like yours. I have tried a lot of options including name selection but has not been fruitful. It will be very much appreciated if you can share your solution to your problem with me. Thank you.

[kaiyeungli]

Hi Andi,

I have use a worksheet defined 'Named Selection'. In the first row of the worksheet, you can see that I add all elements (i.e. elements with ID greater or equal to 1). In the subsequent rows, I remove elements, by ID, where I see fictitious stress concentrations.  

When I look at the results, I then choose 'Named Selection' as the 'Scoping Method' and choose the appropriate 'Named Selection'.

 

Let me know if that helps.

 

Kind regards,

Kai-Yeung

[andimens13]

Thank you very much that worked, however I was also trying to selected  group of elements at various fixing points to eliminate from the stress plot. Using your current method was a bit tidiuos as i had to specify the range or even individual element ID. I have tried to group the elements at the fixing point before eliminating them but i have had no success.Any ideas on that please?

[kaiyeungli]

I agree that it would be a tedious, but that is the only way I know how to do it. If all the fixing points are below an X,Y or Z plane, you can remove the elements based on X,Y or Z location. Just change 'Criterion' from 'Element ID' to 'Location X', but that would only work in certain cases.

[Mike3000]

Another option would be to do the following

1. Select elements to be excluded and assign them to a named selection, e. g. "Elem_excl". The selection can be done manually or by worksheet mode.

2. Select all relevant elements including the ones for which the results shall be displayed and the ones to be removed later and assign them to a named selection, e. g. "Elem_all". You can for example select a body and then convert the selection to meshed elements. This can be done via menu or worksheet.

3. Create a named selection ("Elem_plot") of the elements for which the result shall be displayed. Use worksheet mode: add, mesh element, named selection, equal, Elem_all
remove, mesh element, named selection, equal, Elem_excl

4. Use named selection "Elem_plot" as scope for plotting.