Complex Pocket, create a negative?

[shift1313]

Is it possible to create a solid, that is the negative of an existing pocket or solid feature? I think i can do it by converting a solid to a surface then cutting the surface and closing the bottom( which would be my opening in the solid) but this seems like a very round about way.

 

I dont have an example because someone asked me this question today and i wasnt able to really answer it in an easy way. Things i thought of were copy face, maybe core for mold tooling and what i mentioned above.

 

Anyone done this or needed to do this before?

 

thanks

[JD Mather]

Is it possible to create a solid, that is the negative of an existing pocket or solid feature?

 

There are several methods depending on the design intent and the geometry. As it happens I was working on a tutorial this weekend that demonstrates several methods (sorry this one isn't free).

 

I would always ask the source to supply an example before trying to suggest the best method for a particular case.

[shift1313]

the pocket itself is fairly simple(in his case) just a fairly standard shape with tapered walls. The design intent was to make a negative of the pocket as part of a holding rig(for what i dont know). I think it was more of a general question but i had never come across it until now.

 

how much is your tutorial jd and what is included in it?

 

thanks

[FusiveR]

Figure 1: Before(Above)

 

 

Figure 2: After (Below)

 

Do you seek to achieve what I have depicted above? If so then read on:

 

I will simply list the the steps I performed in order to create the body as shown in figure 2.

 

Step 1: We first create a solid body with a cavity (pocket). In your case "shift" this step should already be complete.

 

Step 2: Now go on to create a "blank". This blank will occupy the same space as the solid body we created above. In my demonstration, I sketched a square with the exact same geometry as the profile of my cavity blank (using convert entities). I then went on to extrude this square so that it now occupies the exact same space (with exception to the cavity) as the cavity blank. IMPORTANT: When extruding or using any similar feature, ensure that merge result is unchecked. You need 2 seperate bodies.

 

Step 3: This is where the magic happens. Use the combine tool (Insert -> Features -> Combine). Select subtract. As your main body select your blank (see step 2). As your body to subtract select your cavity blank.

 

All done.

 

General procedure: Notice how we are simply performing boolean subtraction here.

 

1. We create a body that completely inundates the cavity.

2. We ensure that this is in fact a body. (Make sure merge result is unchecked. The combine feature will be greyed out unless 1+ bodies are present.)

3. We subtract our cavity from the body.

 

Hopefully that clears it up.

 

PS. For further reading (remove all * chars) : ht*tp://ww*w.solidworker.c*om/171/boolean-subtraction-with-indent/

[shift1313]

thanks fusive, the result is exactly what i was looking for. I was hoping to not delete the tool body in the process but that can be handled by saving a non associative copy i guess. I will give this a shot and pass the info along.

 

thanks for taking the time to write that out!!

[FusiveR]

thanks fusive, the result is exactly what i was looking for. I was hoping to not delete the tool body in the process but that can be handled by saving a non associative copy i guess. I will give this a shot and pass the info along.

 

thanks for taking the time to write that out!!

 

No problem.

 

You're not deleting the tool body. It's still very much present. Use the rollback bar to roll up and you'll see it when you pass combine. Feel free to make changes to the tool body and rebuild your document to have the end result updated. Just ensure that the blank always fully inundates the cavity.

[cedar]

I make male/female cavities all the time. I mostly use the surface cut method. Usually I have a “surface master” file and import that to individual part files.

[shift1313]

No problem.

 

You're not deleting the tool body. It's still very much present. Use the rollback bar to roll up and you'll see it when you pass combine. Feel free to make changes to the tool body and rebuild your document to have the end result updated. Just ensure that the blank always fully inundates the cavity.

 

 

the part is still in the design tree but is effectivly "gone" from the model right? Meaning i wouldnt have the part with the pocket and the negative "active" in the model, or is this possible as well? roll back just puts a "break" in the model tree

[FusiveR]

The body is still present in the model, and may be edited.

 

I have created a demo part (remove all * chars): ht*tp://drop.i*o/dtbzaso

 

Modify the dimensions of the fillet in Sketch2@cavity. Rebuild, and witness the change.

 

Is this what you were hoping for?

[shift1313]

not exactly but i was able to do something with your drawing that i didnt think i could do. I selected all the faces of the pocket, and copied them. then i drew a new block, selected a face and pasted and the pocket was created. This allows me to use this new block as the tool body and keep the original.

 

you can see in the image the negative is the part you created, the block i drew next to the original and applied the copied faces to it and voila. that was infinitely easier than i thought.

 

im going to try this on a few complex pockets and see what happens. thanks!