Creating Internal Volume of Part 1

[ME7]

I am interested in calculating the internal volume of a complex shape and use this internal volume of the part to conduct a CFD analysis and calculate its volume. Does anyone know a method to do this? I have been searching for a way to extract the individual surfaces and then to sew them together which can be later formed as volume.
Thank you for help,
Rick

 

[cowski]

First check your CFD package as some have the ability to extract the internal volume for you. For example, CFdesign only requires you to 'cap' each outlet in the model (usually just a simple extrude) and it does the rest.

 

[Guest0527211403]

You can do this with a selection method called "seed and boundary surfaces"

You pick a surface that is part of the set that you want to choose, and Pro/E will keep picking adjacent surfaces until the "boundary" surfaces that you define. The boundary surfaces are NOT part of the selection set.

To use this, first pick a seed surface (so it highlights pink) and then hold down shift and select your boundary surfaces. Then use Ctrl+C followed by Ctrl-V to copy and paste the surface to the same location.

The resulting copied surface is your stitched surface with a bunch of holes in it.

To make a separate volume, there are a few ways to do this.

Make an assembly (i.e. CFD_out.asm) and assemble your part to it. Make sure that it is fully constrained (i.e. no little white square next to the part name in the model tree).

Then create a new part (i.e. cfd_volume.prt) in the assembly (insert-->component-->create) and assemble it to the default location.

Right click this new part in the model tree and select Activate.

Now, while the new part is still active, select your other part with the copied surface in it. Pick the copied surface (whole thing should turn pink) and do a copy & paste again. This will copy the surface FROM that part INTO your new part. This is why the first part must be fully constrained since everything is now relative to the assembly coord sys.

In the copy dialog, expand the options tab and select "exclude surfaces and fill holes". You will then have to pick all of the edges of the holes in your surface.

If all goes well, you should have a closed surface that represents your control volume when you open the part on its own. To find the volume, select the surface and use Edit-->Solidify. This will turn your surface into a solid. If this feature fails, your surface probably has a hole in it somewhere.

Then use Analysis-->Model Analysis-->Mass props to find out the volume.

Another method would use copy geom features, but that requires advance assembly licensing which you might not have.

 

[ME7]

Thank you both for taking the time and effort to respond. I appreciate the input. In the meantime, I will try the method that justkeepgiviner has written and let you know how this works out.

Thanks again!

 

[ME7]

Hi Justkeepgiviner,

I tried the method and I am getting stuck at the point where you mention to select the edges of the hole. I can click on the edge while "exclude surfaces and fill holes" box is still open. I assume the box that saids select surfaces etc is not giving me the feedback that the edges were selected. No new surface is generated at the hole. I tried at both at the part file and assembly file and nothing happens at this stage.

What do you think I am doing wrong in the process?

Regards,
ME7

 

[Guest0527211403]

You might have to click every edge that bounds the hole in the surface in order for it to patch up.

You don't want the surfaces collector anyways, since that is used to exclude surfaces from the copy.

Is you closed volume created by a single part or an assembly of parts? If the latter is true, you might have to do this process for a few parts and merge the surfaces in CFD_volume.prt

Another alternative to filling the holes by copying the parts is to make a new surface in CFD_volume.prt and merge it in.

 

[dgallup]

I have always taken the approach of creating a new "fluid" part and assembling it with the solid parts then subtracting the solid parts from the fluid. One big advantage to this is it can be associative so changes to your solid parts will be reflected in your fluid.