how to calculate the volume change of an object after a pressure simulation?

[Anonymous]

The model I am trying to make is a Gaseous ionization detector which uses a resistive plate chamber. The resistive plate chamber is a made of two glass plates (184.5cmx174cmx3mm) kept 2mm apart using plastic buttons (diameter-10mm and thickness 2mm) and side spacers made of a flexible plastic material (2mm thick). Both the buttons and the side spacer are glued to the glass plates using Scotch Weld Epoxy Adhesive (DP190) glue, so as to support the structure and make an air tight glass chamber (for details  http://www.hecr.tifr.res.in/~bsn/INO/Raveendra-RPC-v3.pdf  ). I made the two glass plates, buttons and the spacer as three different component sets in Fusion 360. I want to make the joints between the glass and the buttons be a adhesive joint and spacer as well.

The study I want to do is for a possible volume change in the chamber if the inside gas pressure is more than the outside atmospheric pressure. But I am finding trouble finding a proper way to select constraints , pressure application and the selection of proper joints in the model. 

After that I want to compute the volume change in the RPC when the simulation is done.

I can't find a way to find the volume of the body obtained from the simulation

 info- http://cms.web.cern.ch/news/resistive-plate-chambers

         http://www.ino.tifr.res.in/ino/theses/satya_thesis.pdf

[John_Holtz]

Hi @Anonymous

We will be glad to help, but we need some more details about:

1. What problem are you having with applying the constraints?
2. What problem are you having with applying the pressure? (My first guess is that is it hard to select the interior face when all of the components are shown. So either hide some components, or if you hold the left mouse button down when over a face, the "select other" dialog will appear from which you can select other faces. My second guess is that the face you selected extends outside the interior of the chamber because you did not split the face so that you can apply the pressure to the appropriate area.)
3. What problem are you having with the contacts?

It may be helpful if you export your model (File > Export) and attach the ".F3D" file to your reply.

Note that the software does not calculate the volume of the deformed model. You will need to do that calculation manually.

[Anonymous]

Hi @John_Holtz

I have figured out how to put on the proper constraints and the proper faces to apply the pressure. The problem is I want the joints between the small circular buttons, the side spacers to be a glue

 joints with the glass plates respectively. Also I want the change in the volume of the setup when the simulation is over.

Akhil

P.S.- I have attached the ".f3d" file for your reference.

[John_Holtz · Accepted solution]

Hi Akhil,

Since Fusion does not calculate the volume of the simulation results, you will have to perform the volume calculation manually by writing down the results and using classical formulas.

I am not sure that you will get accurate results with Fusion because the parts are very thin, and the accuracy of the bending calculation will be important. You probably will not get accurate results with just 1 element through the thickness, and it will be hard to get more than 1 element through the thickness. Modeling the glass plates using shell elements would be a more accurate way to perform the analysis, or the ability to specify 2 or 3 elements through the thickness of a solid is required, but Fusion does not have either of those options.

If you want to use Fusion, I suggest that you take advantage of symmetry. The model is symmetric top-to-bottom, so it can be cut in half through the thickness. It is almost symmetric about the other two planes, so I would use 1/4 symmetry in those directions too. A smaller model will make everything easier: modeling, viewing the model, defining everything, and writing down the results to do your volume calculation. See the attached image "model symmetry.png".

The model is not done solving yet, but it looks as if the contact between the buttons and glass is setup properly. There is no contact between the spacer and the glass because those parts only have line-to-line contact, and contact is not designed for that situation. (See "no contact with spacer.png" and "line to line contact not supported.png") I suspect the real device is held together differently, either because the spacer does make surface-to-surface contact with the glass (so the model is wrong), or there is silicone or other adhesive that "welds" the glass to the spacer (so the model is incomplete).

Let us know what you decide to do.

[John_Holtz · Accepted solution]

Hi Akhil,

I have the results and think that I understand why you think the contact with the buttons are not working. The attached displacement plot shows some nonuniform displacements which would happen if some of the buttons are not making contact. (Let me know if you are seeing something different in  your analysis.)

As you can see in the image, I sliced the model ("Inspect > Create Slice Plane"), and the buttons are bonded to the glass. The reason the displacements are "wrong" is because the mesh on the buttons is different from one button to another. Some buttons have fewer elements, so the cross-section is reduced to a square, while other buttons have more elements so the cross-section is closer to round. The square cross-sections have smaller area, so they are less stiff, than the round cross-sections.

You could select all of the buttons and specify a finer mesh size on them. But given the other drawbacks of Fusion, you may want to consider using a different analysis solution. With Nastran In-CAD for example, you could analyze the glass plates using shell elements (more accurate for bending) and make the buttons from bar elements (don't need to worry about meshing the cross-section). You would still need to perform the volume calculation manually, but the model would be smaller and you could get the displacement results in a text file to perform the calculations.

[Anonymous]

Thanks @John_Holtz

 I got your point about the contact difference between different buttons. I think manual meshing would be a better option. But I do want to point out that the spacer is 5mm in surface contact with both the glass plates.(Attaching the picture herewith)

Lastly thanks for your valuable suggestions and time.

Akhil