Projected holes on curved surface

[Perry_deKruijk]

Hello,

I have an assembly consisting of a curved sheetmetal and 5 sheetmetalparts. 

How can I project the holes in "middle" parts on to the curved sheetmetal?

Notes

-The five connector brackets are in a pattern that follow a 3D sketch with helical curve. 

-I dont care if the hole are not exact circles in the flat pattern eventualy. 

-Unfolding, making holes and refolding is not the way to go i guess; because i want to use the position of the 5 brackets.  

-In the curved sheetmetal part are two bodies; when modelling is finished I will make seperate parts from them. 

Many thanks in advance

[bradeneuropeArthur]

Using copy object may be a solution.

Edit the part in place of the assembly (the parts where you need the holes)

goto the ribbon and Modify tab and choose copy objects.

Copy the 5 brackets

then you can use the brackets as template for your holes position

[kacper.suchomski]

https://forums.autodesk.com/t5/inventor-forum/possible-in-inventor/td-p/12401059/page/2

[IgorMir]

Hi Perry,

I would try to model it as follow:
1. Create an assembly with five parts, placed as needed. Save the assembly.

2. Derive the assembly into a part file. Save the part.

3. Derive the part into a sheet metal part and use its surfaces to build inner and outer shells. 

Cheers,

Igor.

[blandb]

Can you share your assembly

[Perry_deKruijk]

This solution of copy the object in the part is new to me. This might be a good solution for me. Thanks

[Perry_deKruijk]

I have added the files to the original post.

[blandb]

You can copy object and just copy in 1 of the cross braces as a surface to the side rail component. Next, you can start a sketch on the face of the copied object surface and project the edge of the circles and choose to "cut normal". This should cut the circles in and make them circles in the flat. Now, pattern the cut utilizing the same work point pattern.

I noticed that the sides are all 1 solid, but I am hoping this is just for a simplification of this example. To check the flat pattern I had to make the other side rail a separate solid, then used make components to get this one side rail by itself to check the flat.

[SBix26]

Here is my attempt in Inventor 2023 using my favorite multi-body modeling technique.  Since you didn't include the spacer component(?) I made one up.  Any changes you make in the master file (711-3524 - SB.ipt) will be carried through to the components and the assembly.  Change the angle of the spreader holes, for instance, or the hole size, or even the helix pitch or diameter (within reason) -- click Update in the assembly, and everything adjusts accordingly.

Hope this is useful.

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Sam B

Inventor Pro 2025.0.1 | Windows 11 Home 23H2

[Perry_deKruijk]

This looks very good! Thanks for the insights.

The reason I created one part with multiple solids is to keep them adaptive. As you did I wanted to export the solids to separate parts, for production reasons. 

The model I shared is actually simplified, the curved conveyor will have a cross section made up from 16 profiles. (8 stainless steel profiles and 8 plastic profiles) So of course I dont want to change 16 parts as I make a change in the curve size...  

But Im not completely sure if working from one part with 16 solids is the way to go. One part with the 16 solids will be pretty complicated, and a pain in the *** for my collegues to work with. 

It is probably possible to use the same "base sketch" in multiple parts. But I havent dived into this yet... In that case the base sketches will be a 3D for the curve, and a 2d sketch. Any ideas on this..?  

[SBix26]

I'd stick with the one .ipt file with 16 solids.  Naming parameters and solid bodies is helpful for others trying to make sense of the file.  Also, do your colleagues know that they can expand the solid bodies under the Solid Bodies folder and Inventor shows just the features that make up each solid body, so it's easier to find your way?  If it's super complicated, a written guide to the file might be useful for others trying to edit it.

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Sam B

Inventor Pro 2025.0.1 | Windows 11 Home 23H2