Surface projection on curved, slanted surface?

[tramtin]

I've projected a sketch on to a slanted, curved surface and I want to depress that design. 

Am I right in thinking that this is impossible to do with Fusion? Is there a workaround?

Extruding the original sketch on to the surface would not work for me, as the indentation would be shallow towards the edge but much deeper towards the center.

[TheCADWhisperer]

@tramtin 

Now add a 11.5 Fillet to this edge.

Drag the Timeline Marker back to the end of the history.

Verify that the Shell doesn't fail.

Drag the Timeline Marker back in history to before the Mirror feature.

Add the smaller fillets at the top.

Repeat the test.

Attach your progress file here.

[tramtin]

Here's the file for step one. I note that your design has the bottom and top lines shown as the diameter, whereas mine shows only half (30cm vs 15cm, for example). Have I overlooked something?

[TheCADWhisperer]

@tramtin 

Check back in a while for a video.

[TheCADWhisperer]

@tramtin 

[tramtin]

I've cleaned up the design as per your video and continued with message no. 20. File attached. I think I got it right, so I will proceed.

[tramtin]

And here's the file with added fillets, as instructed in message no. 21.

[TheCADWhisperer]

@tramtin 

Now Edit Sketch1 and add a 3-Point Rectangle...

Sketch the 3-Point Rectangle snapping two locations on the angled line (be careful not to snap to the midpoint of the original angled line).

Add the 3 dimensions. (You can alter later as desired.)

Zoom in on the image above to enlarge the view.

Drag the Timeline Marker back to before Mirror.

Revolve-Cut the 3-Point Rectangle (I am showing Edit rather than Revolve because I already did it).

Drag the Timeline Marker back to the end and check the Shell.

Drag the Timeline Marker back to before Mirror and add the Fillets. (The order in which you place these Fillets is critical to how they look aesthetically.  I would probably do the short corner lines first,) You can try different orders.

Drag the Timeline Marker back to then end and check the Sell.

Doing the similar features on the top will be a little different sequence of steps.

Attach your progress file here.

[tramtin]

File attached.

I think it's going well.

[TheCADWhisperer]

@tramtin 

Making good progress. 

The next few steps might seem confounding at first, but just follow along and it will quickly make sense...

Edit Sketch1 and Mirror the angled rectangle about the vertical centerline.

Click on image above to enlarge the view.

Drag the Timeline Marker before the Mirror Body.

Revolve - Cut the mirrored rectangle by 48°about the Z axis.

DO NOT ADD THE FILLETS YET.

Do the usual tests of the Mirror and Shell.

I have to join the wife for dinner, check back later for next set of steps.

[tramtin]

Ok, I've done that. I think you meant to say to cut the mirrored rectangle by 24°, as the resulting cut with 48° is too large.

[tramtin]

[TheCADWhisperer]

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@tramtin wrote:

Ok, I've done that. I think you meant to say to cut the mirrored rectangle by 24°, as the resulting cut with 48° is too large.

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@tramtin 

Nope, as I said, my instructions might initially seem to not make sense.

Do the Revolve - Cut as 48°.

[TheCADWhisperer]

@tramtin 

Now do a Revolve Join by 36°

Now do a Revolve Cut by 33°.  (We can adjust all of these dimensions later as desired.)

Do another Revolve Join by 21°

Now do another Revolve - Cut by 18°

Hide Sketch1 and test the Mirror and Shell to make sure they don't fail.

You can add the fillets to the center slot, but not to the two (four) end slots yet.

You can Edit Feature and adjust the angles as needed. (I don't have the part in hand and calipers to check.)

[TheCADWhisperer]

@tramtin 

Before we put in these straight ribs, can you take a couple more pictures closer and at different angles?

I am not sure of the geometry. (visualizing without the fillets)

Edit:
BTW - someone might jump in here and admonish that we have introduced an undercut.  Don't worry observant folks, we will take care of that later.

This wouldn't release from an injection mold but probably doesn't matter for 3D printing.  We will address the issue anyhow.

[tramtin]

Ok, that's done.

More pictures of the ribs attached.

One thing to note is that all the ribs, including the first and the last, are straight. The indentations are 3mm deep.

[TheCADWhisperer]

@tramtin 

I need to ponder a bit on the "best" way to create these ribs.

I have an idea but need to experiment first.

Check back later.

[tramtin]

Thank you, yes, I will stand by. Maybe it's nice for you to have been presented with a little challenge after all?

Thank you so much for all the help you've already given me. I didn't expect this and I appreciate it very much!

[TheCADWhisperer]

@tramtin 

As I was testing out my "solution" for the straight ribs I noticed that you dimensioned this 3mm as vertical dimension when it should probably be aligned dimension.

[TheCADWhisperer]

@tramtin 

This turned out to be tricker than I expected, but we will get it done.

Here is image of my "solution" without the fillets.

When I start making edits - often it confuses beginners.

Edit the first Revolve we did at the top to 21°.

Delete the other Revolves that we did at the top.

[TheCADWhisperer]

@tramtin 

Edit Sketch1.

Mirror the longer angled line.

Sketch new parallel line in space (shown red in image).

Make the new sketch line = (Equal Constraint) to the mirrored long line.

Add a Midpoint Constraint between the newly sketched line and the bottom line of the rectangle.

Should automatically be parallel, but add that constraint if missing.

Your result should look line this (no blue lines or white endpoints).

Attach progress file here for next step.