Projecting a drawing onto a complex curved surface

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1

I’ve seen similar topics but none of the directions work for me. I have an object with many different curves making up it’s top surface.

I have a drawing above it that I want to project onto the surface and then extrude only the part of the drawing inside the perimeter down into the object just a small amount. Crucially, the bottom of the extrusion needs to follow the surface contour of the part, not have a flat bottom.

My understanding is that I need to select the drawing, click project, and then select the object. But when I try that I just keep getting “Something went wrong but your project is intact”.

I can’t get to the step of figuring out how to extrude the drawing down into the part following the surface contour, because I can’t get even the drawing to project onto it.

Please, please if someone could walk me though this like you would with a 5 year old I would be eternally grateful.

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2

Can you share the project?

3

I will share it this evening. What’s the process for that?

There are an embarassing number of different drawings, fillets, chamfers, and other things that I did to force this thing into the shape I wanted. Some of the items on the long list of things I did have an error mark on them.

It’s possible that I’m doing the right thing but the project is a compromised by something. I guess could export and then re-import it “clean” as a STEP file and retry it that way?

4

Export it as a .shapr file and send it in any convenient way.

Could be.

I don’t think that will help but you can try.

5

Sent. Thanks for taking a look at this!

6

I just want that drawing to extend down into the top of the part about .01 while following the precise contour of the top of the part. I’m trying these steps (see below). I THINK I’m get through step 2 successfully but then can’t get any further. There doesn’t seem to be a way to select the entire face of my my object. I can select only one little piece or “facet” of it.

Step

Action

Description

1. Create Your Sketch

Create a construction plane above your object and draw the 2D sketch that defines the boundaries of your desired feature.

This is exactly as you described in your question.

2. Extrude the Sketch as a New Body

Use Tools > Add > Extrude on your sketch. Extrude it downwards so that it completely passes through the top surface of your irregular object. Crucially, ensure this is created as a New Body, not joined to the existing one.

You now have two separate bodies: your original object and a new “tool” body that represents the volume you want to work with.

3. Select the Bottom Face (or is it the top face?)

Tap to select the flat, bottom face of the new “tool” body you just created.

This is the face you are going to replace.

4. Use the Replace Face Tool

Go to Tools > Replace Face.

This tool is designed to extend or trim a body by replacing one of its faces with another surface.

5. Select the Target Surface

The tool will prompt you to select the target face. Tap on the irregular top surface of your original object.

Shapr3D will now calculate the intersection and trim the bottom of your “tool” body so it perfectly matches the contours of the irregular surface.

6. Perform the Final Operation

You now have a “tool” body that is perfectly shaped for your operation. Use Tools > Subtract to cut this tool body from your original object. If you wanted to add a feature instead, you would use Tools > Union.

This will leave a pocket (or an embossed feature) where the bottom of the pocket has the exact same curvature as the original surface.

I’m stuck on this part:

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7

Getting closer? Using the steps above creates a reversed convex surface to my “tool”, but what I want it to do is create a tool with a concave surface that I can then extrude or push down into my part a little bit that follows it’s upper surface exactly.

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8

Well I kept at it and finally got it. This is what worked.

Re-Extrude the Tool as a Solid Block

Start by ignoring the shell you currently have and use your original flat sketch to make a solid tool.

  • Step 1: Select the original closed sketch profile you used to make the tool.

  • Step 2: Pull the extrusion arrow to push it completely through the complex upper surface of your main object.

  • Step 3: A box with a boolean badge will appear. Change it to “New Body” and hit Done. You now have a solid block intersecting your object.

:two: Imprint the Complex Curve onto the Solid

Now we use your main object to shape the bottom of this new solid tool.

  • Step 4: Navigate to the menu and select Tools > Subtract

  • Step 5: Tap your New Solid Tool as the body to be modified (highlighted in purple).

  • Step 6: Tap your Main Object as the removing body (highlighted in blue).

  • Step 7: Look at the menu on the left and toggle Keep Originals to ON

    (Keep removed items)

    (This is the most critical step so your main object doesn’t disappear!)

  • Step 8: Tap Done.

:three: Lower the Tool and Carve the .01 Pocket

Your solid tool now has a bottom face that perfectly matches the complex curve of your object. Let’s make the pocket.

  • Step 9: Select your solid tool in the workspace.

  • Step 10: Tap the Move tool, grab the arrow pointing straight down, and move the tool into your object by exactly .01.

  • Step 11: Go to Tools > Subtract again.

  • Step 12: This time, tap your Main Object as the target (purple) and the Lowered Solid Tool as the removing body (blue).

  • Step 13: Make sure Keep Originals is turned OFF this time so the tool deletes itself. Tap Done.

It was so I could push a shallow pocket into the part, select only that pocket, and apply a texture so I’d have an untextured border around the part.

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9

Glad you managed to do that yourself. Just in case, here’s a video showing how I would do it.