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.
Yes, leave the old mirrored Rectangle there - we will still need it.
It is OK that the mirror of the longer line is over the Rectangle.
It is OK if there are no black dots, just no white dots for sure at the ends of the lines.
I post next step....
I just realized that I had you do extra work - we could have done the same line on the original side of the sketch without Mirror.
Move the Timeline Marker to just after the Sketch1.
On the Surface tab (we haven't used these Surface tools previously) Revolve the lower line around the axis.
Create a Plane at Angle of 90°to the top line.
This is getting complicated enough that I might have to make a video of these steps.
You have it.
Now hide the visibility of the solid body.
Drag the Timeline Marker to just before the Mirror.
Start a New Sketch on the angled work plane.
P on the keyboard for Project (geometry)
and select the top SHORTER LINE of the Rectangle. (Because there are two lines overtop of each other it might be difficult to select the correct (shorter) line. If you hover the mouse over the lines a selection box will appear that will let you select the shorter line from a list.
Hide Sketch1.
Sketch a line to the right of the Projected line in Sketch2.
1. Dimension the length of the line as 30mm.
2. Dimension the vertical height of the line from the top endpoint of the Projected line as 8mm. (You might have to drag the line roughly into position after adding the 30mm dimension).
3. Add a Coincident constraint be select the Vertical line and then Shift select the Midpoint of the Horizontal line. This will move it over onto the Projected line.
Now double click on the 8mm and change to 0.8mm (we could have done this first, but I wanted it to be clear we are not on the endpoint).
Click on the Projected line and hit x on the keyboard to convert it to Construction linetype (I hid the surface body to make this image a bit more obvious.
Click on the image above to enlarge the view.
Sketch two angled lines approximately as shown and add 12° dimension.
Add a Horizontal line and add Coincident endpoints to the two angled lines...
Now add a Midpoint Constraint between the Horizontal line and the endpoint of the Projected line as shown below. Everything turns black.
Finish Sketch.
The next few steps might be tricky as likely the first time you have used Thin Feature.
Select the Extrude command and select the Thin Feature option to the right at top of dialog box and UNCHECK Chaining.
If the inside profile is still highlighted - click inside the profile to unselect.
Now select ONLY the top Horizontal line.
Select the To Object in the Extant Type and then click on the Revolved Surface Body.
DO NOT ENTER a distance - Fusion will do that for you automatically when you select the Surface.
Set the Wall Thickness to 2.75 going down (probably Side 2, but this might very depending on how previous geometry was created - the key is the thickness should be on the bottom side of the line as in the image below).
Click OK.
Now select Rectangular Pattern command.
Set the selection to Bodies and select the extruded body as the Object to pattern.
Select Axis and select the vertical Construction line.
Set the Distribution to Spacing and enter 15 Copies at 5mm Distance spacing.
Click OK.
Now select Extrude again.
Set to To Object and select the Revolved Surface body.
Do not need to enter a distance - Fusion will do that for you.
Select the Extend option as indicated. (or we could have opted for Through All)
Set to INTERSECTION. (Very few designers in an CAD software make use of the Intersect option.)
We better stop here and check progress before next set of steps.
Attach your file here.
In the next set of steps we are going to appropriately use the Move command which is almost always the wrong move for beginners (as they use it).
When we Extruded these ribs to the Surface Body the bottom of the ribs follow the contour of the Surface Body cone. Subtle, but important.
Whenever I say terms like Horizontal (especially if I capitalize) or Vertical or Tangent or Equal or Parallel or Perpendicular I am referring to absolute geometry constraints.
For the next few steps I turned off Display Component Colors that somehow got turned on.
Instead, I assign Appearances.
This doesn't really matter though.
Select the Move command (I almost never advise beginners to use Move as they use the command in inappropriate circumstances).
You can Window select (from left to right) of the "rib" bodies to Move/Copy(Rotate).
Select Rotate option and select the Z Axis as the axis of revolution.
Enter -45 and select the option to Create Copy.
Click OK.
Select Move (Rotate) but no copy as -30
Now select the Combine tool
and set to Subtract...
Select first the main body and then Window select (from left to right) the bodies to subtract.
Click OK (we will go back and add Fillets to the ribs later).
As usual, test the Mirror and the Shell.
Yippee! That worked!
But my goodness, I would have never figured out how to do this. No amount of trial and error clicking would have got me there. I'm in awe, thank you!
Edit Sketch1.
Add this short Perpendicular line inside the Rectangle.
With the Timeline marker AFTER mirror but before Shell, Revolve inside the Rectangle as shown as New Body.
Move Rotate the new body around the Z Axis by -90 degrees.
Combine - Subtract the new body.
You see how we used the history timeline. We don't want this feature mirrored so we did it after mirror, but we do want it shelled.
Next set steps to follow.
Challenge - see how @davebYYPCU created the spherical "Rivets" back in Message #11.
Rivets added. The copying process can most likely be better automated, but it looks like I got there in the end.
Question: Should I 'Combine' the rivets with the body?
