I should calculate the variation of the area of a hole made on a pressure pipe (HDPE).The piping is deformed due to pressure.
The hole passes from circular to elliptical.
How can I calculate, on Mechanical, the area of the elliptical hole?
Dear Colleagues,
I went through all the answers and actually I liked the idea from Claudio Pedrazzi
where we can export displacement contours and do the curve fit and finally estimate the surface area. However, there is another method that you can easily measure the deformed surface ANSYS WB via Mechanical that I want to share with you.After you did your analysis in “Static Structural” module (let’s call it main module), insert another new “Static Structural” module beside it. Then, transfer the “Solution” of the main module to the “Model” section of the new module that you just inserted. Double clicking on the “Model” enables editing the deformed geometry from the main module in the new module. From “View” “Windows” activate “Selection Information” pane. Now you can select deformed surface that you are interested and check the result for area in the “Selection Information” pane. This method is quite useful and saves lots of time.
Good luck,
Claudio Pedrazzi
Unfortunately I have no idea how to project the points on a plane. Is there a way to export the deformed 3D model and measure the area on AutoCad?
I found this thread using google search and checked it in Ansys. it works.
https://www.eng-tips.com/viewthread.cfm?qid=443416
This was for measuring the contact area. I guess you can modify and use it for measuring the area. Thanks for asking this question. I learnt something today.
Hi Mr. Claudio Pedrazzi , in that case perhaps that dummy shell elements (of negligible thickness) representing the hole can be created and their area can be measured. But of course, it should have no external loads acting on it.
If I understand correctly, the hole has 3D curvilinear boundary and it is difficult to say what is its area, especially after deformation. Fortunately, Claudio Pedrazzi
has proposed to project it on a plane. I think that it is not difficult to code the next algorithm. The plot in the hole.bmp should clarify the calculations.
Dear Colleagues,
I went through all the answers and actually I liked the idea from Claudio Pedrazzi
where we can export displacement contours and do the curve fit and finally estimate the surface area. However, there is another method that you can easily measure the deformed surface ANSYS WB via Mechanical that I want to share with you.After you did your analysis in “Static Structural” module (let’s call it main module), insert another new “Static Structural” module beside it. Then, transfer the “Solution” of the main module to the “Model” section of the new module that you just inserted. Double clicking on the “Model” enables editing the deformed geometry from the main module in the new module. From “View” “Windows” activate “Selection Information” pane. Now you can select deformed surface that you are interested and check the result for area in the “Selection Information” pane. This method is quite useful and saves lots of time.
Good luck,
Dear Claudio Pedrazzi
,Your very welcome. I knew that you may like it!
By the way the thing that you mentioned about “Scale Factor”, I was not aware of it till now and learned something new too.
I’m totally agree with you. Every time I contribute to RG community, I learn something new and this is fantastic.
We have one expression in our language which says “The tax of knowing something is sharing it with other people”. Hope all of us can keep up with what we are doing right now for a long time.
Regards,
Dear colleagues,
I decided to verify the idea about modelling of the hole by dummy elements. For this purpose I considered clamped shell with two holes (1/8 symmetrical part) under internal pressure. I modelled the hole by shell elements with very soft material (10-16 of shell Young's modulus). As was expected, the results depended on thickness of dummy elements. The file hole1.png shows results for different h1/h0, where h0 and h1 are the thickness of the shell and dummy elements correspondingly. The stress distribution for all three cases was the same and coincided with the results for real hole. We can see that bending of the soft part has its own logic, and it is not clear which thickness of dummy elements should be selected to calculate the hole area variation.
I am sure that this approach is good for plane and axisymmetric problems where only in-plane deformations take place.
- Badges
- Science topic
- Similar topics
- Thermodynamics
- Pressure