🎉Community Raffle - Win $25

An exclusive raffle opportunity for active members like you! Complete your profile, answer questions and get your first accepted badge to enter the raffle.

Join and Win

Pressure to elements

Altair Forum User

Is there an easy way to apply pressures to elements when there is a varying load across the surface.? Right now, I have to select which elements I want for a given magnitude to apply the pressure, as well as nodes for the normal face. This is extremely time consuming considering I'm running multiple different cases. Additionally, if I remesh or open a new model, I have to do the same process over. If there was a way to copy a load from a different model or import a spreadsheet that would be awesome and save me a ton of time.

Thanks

-Dave

Find more posts tagged with

English

OptiStruct

Accepted answers

All comments

tinh

Hi,

with varying load on element you can switch 'magnitude' to 'equation'

forexample you enter 'z' means p = z so pressure varying along z coordinate

reference:

http://forum.altairhyperworks.com/index.php?/topic/9038-how-to-apply-variable-pressure-on-a-curved-surface/

Altair Forum User

Hi Dave,

Please refer to the chapter 'Boundary conditions and Loads' in Practical Aspects of Finite element Simulation for information on how to apply varying pressure.

You can order for free E-book from http://www.altairuniversity.com/free-study-guide-book/

Rahul_P1

I suggest linear interpolation in the pressures panel, this will let you apply pressures from a .ssv file

4 values are required in the file, which are:

So, you could have a file that looks something like:

0.500 0.500 0.000 1.000

3.500 0.500 0.000 4.000

3.500 3.500 0.000 8.000

The resulting pressures are created normal to the elements.

There is a way to transfer varying pressure from one model to another as below,

1. On your currently meshed model go to the Morphing pulldown

2. Select Create>Shapes

3. Go to the convert sub panel

4. Select the Pressures to shapes option and pick your pressure load collector and click convert

You will see arrows representing the shape on the nodes. It will average the pressure to the nodes

5. Click the Save/load subpanel below convert and select the save shapes option

6. Click browse to indicate the location of this file, select the newly created shape, make sure the option below is set for 'as shapes' and click save.

7. Delete your pressure load collector and remesh your part

8. Go back to the save/load subpanel and select load shapes.

9. Browse to and select the shape file you saved in step 6.

10. Make sure the 'apply shapes' box is DESELECTED! (this is IMPORTANT) and click load.

11. Go back to the convert subpanel and pick the shapes to pressures option.

12. Pick the shape and convert.

13. It will average the values on the nodes to create the proper pressure on the element.