How do I make a pocket with a variable depth ?
I tried to do this with a 3D sketch, but it's to difficult to position it right and dimension it right.
How would you do this ?
Is the green image what you are trying to achieve? Because that just looks like a straight extrude cut.
If by variable depth you mean sloping at an angle, then you could draw a 2D sketch on one of the vertical faces or planes, depending which way it slopes, & then extrude cut.
EDIT: OK, I just noticed the subtle differences in the corner heights, I assume that's from the top surface? What you've done seems fine, you just need to fully define it & then extrude cut in a direction.
Add two planes perpendicular to the top where the edges of the pocket will be. Add a line to each plane to establish the edges. create a surface loft between the two, extrude cut to surface from the top.
I would use a 2D sketch and the sketch plane would be the top of the pc and use a Cut Extrude for your depth..
How will that achieve the varying heights at each corner of the pocket?
Thanks for catching that Bjorn Hulman
I totally missed the four dimensions being different. Ok so using the sketch that is shown, you can create a surface there and use additional surfacing tools to split it, then delete the appropriate faces..
Sketch on your face as usual.
Use a 3d sketch to define 3 points (along axis with corners of sketch) and dimensioned from same.
Create a plane from these points, cut upto surface
Bjorn, I like your thinking. Did you know you can do the same thing you've suggested but without the surface loft? Oddly enough you can pick a plane just as easily as a surface to extrude to. So if you were to draw a line to represent the taper you need in the pocket, then create a plane coincident with that line you're done. That is of course assuming that the pocket is just tapered from side to side. If the pocket has four different corner depths then your solution would be key. Never knew that until one day I was just messing around trying to break SW ... lol
The 4 corner points of the pocket are on the same plane, so I would do as folllows:
1) sketch 3 of the 4 corner points using 2 separate sketches or 1 3D sketch
2) build a plane using 3 of the 4 corner points
3) Then, if the pocket needs to be perpendicular to the top face then use "extrude cut" from the top face using the option "Up To Surface" selecting the plane just built. If the pocket needs to be perpendicular to the pocket face then use "extrude cut" from the plane just built up to all.
Hi John Pesaturo,
I was looking at the sketch of the first image provided, and made a quick assumption that the depth dimensions of the corners were of a precision that had importance. I also assumed that all 4 of those corners were unlikely to share a planar relationship so the surface seemed like a good idea. I was aware you can extrude up to a plan, but mentioning it for others to read is always good.
With the 4 corners being different that creates a twisted surface, you could still create the sketch like you mentioned and then add the 3D sketch and add the (4) four points in the corner by adding relations, or you could use just short vertical construction lines that would be in the Z axis and would have the depth dimension and then you could draw a line from corner to corner and do the loft that Bjorn Hulman mentions..
Sorry Rob I didn't see your answer before I gave mine!!! I would have done the same.
I made a quick attempt.
Rob Edwards wrote: How about? Sketch on your face as usual.Use a 3d sketch to define 3 points (along axis with corners of sketch) and dimensioned from same.Create a plane from these points, cut upto surface
Rob Edwards wrote:
Or do 1 point in the 3d sketch and extrude up to vertex. But if you want the floor of your cut to be angled, then your way would be better.
Just what I was going to say Rob! If I can complete my thoughts I would have added, put the dimensions of those points in an Equation and create a plane. Someone already suggested a plane though.
If it's planar it would be easier, three different points suggests it isn't planar though.
It was the forth that lead me to assume it wasn't planar.
I reread John's comment and missed it, Thanks!
Yes, I missed that as well.
Another option would be to mode a solid body with that shape, then use it as a cutting piece to produce the cutout that you want.
Good one Dan! Off the top of my head I don't recall, does that operation allow linking to a file or only the inserted one?
You could do it a few different ways:
1) Create the solid shape in a different part and bring it in to make the cut using the "Insert"-->"Part..." function. (this would link the two parts together)
2) Create the solid shape inside THIS part on location and don't merge Bodies, then use it to make the cut.
3) Create the solid shape inside THIS part at the origin in whatever orientation you want and then use the move body to get it into position and then make the cut.
4) and now that I have played with it, really the way I would do this is the use of "Thickened cut". Use your 3d sketch to create a fill surface and then use thickened cut to cut it away. (see attached video).
And then I realized that the walls of the thickened cut would be perpendicular to the surface, which is twisted....which would make it extremely hard to machine.
SO, here is another method of doing the same thing. Just a simple cut extrude with direction to make the walls of the cut perpendicular to the face of the base plate.
See attached video.
I think we're back to the created plane and extrude cut perpendicular from there to avoid machining issues. 5 axis required!
Always good fun exploring the many ways, how about a boundary cut?
Hard to see from the image - is the bottom taping down? if so, then just apply draft to the bottom face
See Wayne's attachment
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