SOLVESPACE -- parametric 2d/3d CAD

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Blind tapered hole possible? (by Michael)
Is it possible for SolveSpace to design a blind tapered hole?

If so, can someone advise the steps to design them?

Thank you, in advance!
Sat Dec 22 2018, 22:50:35
(no subject) (by Andrew)
Sketch a half section of the hole in a plane through its center line, and lathe it to create the hole. (Difference is an option with Lathe.)
Sun Dec 23 2018, 08:28:48
(no subject) (by Michael)
Yes, I see how your advice would work for a blind central hole on axis. I should have been more specific, forgive me. What I need are 6 blind tapered holes, .300" deep arrayed on a 2.75" circle. Thickness of material is .900". Can that be designed in SolveSpace?
Mon Dec 24 2018, 18:45:23
(no subject) (by Andrew)
You can create a circle, and make it a construction circle, to place your hole circle, and position a point of this circle to create the sketch plane for the first hole(select the point and orientate you view to close to the desired plane to create a sketch plane). You will want to wire frame the body so you can see what you are doing. Lathe and the step translating to create the array of holes.
Mon Dec 24 2018, 20:03:05
(no subject) (by Michael)
Hi Andrew - I understand creating an array of holes all the same diameter and depth. I do not understand how the holes would or could be tapered, wide (say .500") at the surface and smaller diameter (say .375") at the bottom of the hole at a depth of .300".

Thank you for replying. Is this possible?
Tue Dec 25 2018, 18:40:25
(no subject) (by Andrew)
You can array the result of a lathe operation, which gives you the tapered hole. You can draw a circle on your solid, and make it a construction circle. You can use a point on that circle to anchor a plane to draw the hole half section, lathe it to create a conical hole, and array that round the circle to give the array of holes round the construction circle.

There is a video dealing with step rotation in the tutorials, but rather than extruding a circle, you will have to lathe a drawing to meet the taper requirement. To see what you are doing in drawing this on a a plane inside a solid, turn on wireframe mode while making the section drawing, (right hand icon), so that you can see the drawing. The lathe operation allows it to be a difference operation, and to see the result you may need to "force NURBS to triangle mesh".
Tue Dec 25 2018, 19:44:46
(no subject) (by Paul)
I tried this with success but it was tricky.

1) draw a circle in the location of the hole prior to extruding the part.
2) make that circle a construction line.
3) draw a radial line segment from center to perimeter and make that construction as well.

4) After extrusion, find the option to hide shaded surfaces - it's one of the little icons at the top of the text window.
5) Select the radial line, the axial line at the center of the circle, and the point where they meet. Then sketch-in-new-plane. This will align the view to the cross-section of your hole.
6) trace the radial line, the axial line, and the rest of the hole profile. These are real lines this time, not construction lines.
7) lathe. then check difference for the group to cut it out.

I also had to convert to triangle mesh for this to view properly. Oh and undo step 4 to see the solid.

Not sure if this is a more or less useful description.
Wed Dec 26 2018, 09:22:53
(no subject) (by Michael)
Andrew and Paul - THANK YOU! Following and interpreting both of your suggestions, I've gotten it to work! Being new to 3D CAD, I probably come across as hard headed or stubborn, I apologize if I do. I'm really not, I am struggling to understand HOW TO USE the software to draw what's in my head.

Thank you for your patience and persistence!

I wish you both a very Happy New Year!
Wed Dec 26 2018, 11:26:04
(no subject) (by Paul)
@Michael you're welcome. This was new for me too! I just followed Andrews instructions but realized some of the details might not be very obvious so I tried to make it more explicit. I had even tried to do something like this before with no luck.
Thu Dec 27 2018, 09:15:13
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