Projected punched hole on arcs

[onefjef]

I have a cylindrical housing with a 2" wide mounting flange around the perimeter. There is a part that needs to mate to the outside of this with a similar flange. I have the punched hole pattern in the first housing flange and I would like to know if there are any tricks to projecting the punches slot positions from first to second flanges. I only have (6) holes in this case and could create a work around but if a person had many many holes then a more streamlined, constrained approach would be needed. Could someone please suggest a work flow for this?

 

[mcgyvr]

Not sure if I follow you exactly.. but you can put both parts into an assembly and constrain in place and then edit the one without holes and project holes from the other part.
Note!! to edit a part in an assembly that part cannot be open in Inventor at that time.

 

[onefjef]

mcgyvr,
I will attach some PDF images of what I'm trying to accomplish. As you can see I do have a work around. I started with the outside rolled flange with slotted holes. I added the inside flange without holes. I wanted to create slotted holes on the inside flange that lined up with the outside flange.
I know about in place editing but in order to project from part to part I would need to create a sketch plane for each hole tangent to curve. Sounds like a lot of sketching to me.

Work around:
1. On the inside flange band create midplane sketch. Project edges of outside band slotted holes onto sketch. For each projected edge: Create construction lines through arc center and ending at midpoint of projected edge (perp). Draw rectangle shape connected to end of contruction line at projected edge and make bottom perpendicular to construction line.
2. Create a midplane cut using the rectangles. This is done just to mark the location of the holes.
3. Now unfold the inside flange band.
4. Create a sketch on the flattened face. The cut created will indicate where I need to locate and constrain some circles to be used for the sheet metal punch tool in the next step.
5. Use the Punch tool with the circle centers.
6. Refold the band. You can see the holes line up.
7. Done.

http://files.engineering.com/getfile.aspx?folder=3398b409-35e3-43c6-a250-25b873daff14&file=BANDS.pdf

http://files.engineering.com/getfil...-5d65-43aa-814a-79c0b0756453&file=BANDS_2.pdf

I'm open to more streamlined approach.

Thank you.

 

[EngAddict]

I might create it something like the attached picture.

1. Create your curve as a surface
2. Create your 2D sketch of the slot and hole on the surface
3. Use a 3D sketch to wrap it to the surface and split the face
4. No derive into parts and thicken one band in one direction and the other band in the other direction or create a multibody and push the solids into parts files (depending on release)

You can create offset surfaces for the correct mid-plane if you want it exact, or leave the hole out of the split and add if later, thicken one from the other (not the surface), you could place an ifeature for the slot and a hole on a point to create the two features, etc. There are may different ways to do it. But basically I would always use a reference part instead of a adding it in the assembly edit.

 

[onefjef]

This sounds like a very clean method. Thank you.