Chamber Volume

[n18h7m4r3]

Hello,

I am modeling a gear pump and want to calculate the chamber volume enclosed by the gear housing and the two gears at discharge port. I have looked around for this at many forums but none were of any help.

Making a Cutout with a solid gear pump model (with no cavity inside) doesn't helps as it creates volume between gear teeth and pump house also which are not at discharge port.

My requirement is only for that volume which is enclosed between the two gears and pump house near discharge port.

Here is a sample picture of gear pump http://gearpump.co.jp/english/main.files/pump01.gif

Thanks

 

[design-engine]

I use top down design for this type of thing. Surfaces in a copy geometry add or subtract material then convert mass props to volume

 

[n18h7m4r3]

Hello Bart,

I didn't follow you with your answer. Can you explain in detail as I am not an advanced Pro/E user. Do you mean that I should make a new solid model using the enclosing surfaces? If yest then how?

Thanks

 

[Jacoolo]

you could make a Save a copy > Shrinkwrap > with Auto holes filling.

This should give yoy whole assembly as one part filled inside. With this is your assembly, You can cut out housing and the rest of needed part to achieve what you want

 

[jimshaw]

nightmare,


assemble or insert a new empty component into the assembly. Activate it and create copy geom (insert>copy geometry). Now select the outer surfaces of the parts that make up the walls of the volume that you are trying to aquire. This creates a copy geom feature in the model tree of your new part. Insert copy geom for every unique part in the assy. Now open the new part and manipulate it until you have isolated the volume you want. Once you have the desired volume bounded by surfaces, merge, trim and solidify.


If you need more detail, you'll prob have to start sending us screenshots or the files. The best part is it's all parametric, so any changes that occur in the assy will be reflected in your new part.


Hope this helps!


Jim

 

[n18h7m4r3]

Hello Jimshaw.


I cannot select surfaces from different parts in an assembly to create a volume. Is there any other way to that?

 

[Jacoolo]

you`re not able to pick in one set surf from different components. You should do this as separate steps and then in end model merge them. This is fine appraoch to achieve what You desired, but if I were You, I would follow my way - Shrinkwrap, and cut out, less clicks, and less tweaking with surfaces which can in the end runs crazy

 

[n18h7m4r3]

The problem with using shrinkwrap is that I get other volumes also which I do not need, like the volume between gear teeth and other holes in the pump housing.

 

[Jacoolo]

exactly, but then Uou just put shrinkwrap in your assembly, active the intresting, active amd make a cut out with this you gonna cut inner volume

 

[jimshaw]

nightmare, please send us a snapshot so we may help you at a higher level.

 

[n18h7m4r3]

Hello Jimshaw,

Attaching a photo of a basic gear pump. My aim is to estimate the volume between two gears (green) and the oval pump housing (blue) (there are two such volumes in this snap).



This volume changes as the gear rotate and I will need to calculate this volume for this gear positions.

 

[jimshaw]

Is the red volume what your after? What is happening at the part interfaces where the blue arrowsare pointing. Do the gears touch and make a PERFECT line?

 

[n18h7m4r3]

This is exactly the volume of my interest and yes gears do touch with gear housing and do not interfere.

 

[jraquet]

If it is only the red area can you not make a part in the assembly, use the edges of the parts (the red lines) and then an extrusion of the captured cross section?

 

[jimshaw]

Nightmare,at this point, it is obvious to me that a handful of top-down modeling techniques are available to you, are you looking for the exact button clicks to do this? As jraquet implies, the resulting volume has a constant cross-section so something as simple as creating a new part and copying the curves for use in a protusionwould work just fine.


Have you been able to create a new empty part in your assembly and activate it yet? Do this, then use copy geom to copy the surfaces (for example) from each part in the assembly. The result should be 3 separate features in your new part. Now, merge the surfaces together by selecting the two adjacent surfaces and using edit>merge. When complete, the resultant quilt should already be prehighlighted, and now select [ctrl] and the third adjacent surface, and merge these together. Keep doing this until you have 1 quilt. Now cap the front and back openeings with a surface. This can be done with a sketch, use the edges of the existing quilt to create the outline, and then fill the sketch in. Two more merges should give you a completely sealed single quilt volume. Now highlight that and select edit>solidify. Now you have mass in the model, and you can perform mass properties, such as volume.


The new volume should be parametric as well, so you can rotate the gears and everything will update. Keep an eye on the "use edges" in the sketch, as they may get broken. Let me know how this works out...

 

[n18h7m4r3]

Thanks a lot Jimshaw and Jraquet, I am finally able to do what I intended. Its really a breeze now with your help.

And Jim, the volume is parametric but as long as the surface making the volume remain same (which however change for some angles of gears) but that is not a problem. Now I can complete my work with no difficulty.

 

[jimshaw]

Great news, glad to help. Yes, I believe it is very difficult for ProE (or any CAD tool for that matter) to keep references when the number of entities changes. Especially with edge references...