Extruding angular object into block

[Zerb]

im going to try and explain this the best i can here in order to hopefully get helped towards a solution.  im trying to lay out a bit holder, unibit drill bits to be exact, that i will 3D print.  i dont want anything fancy, just made a rectangular block and i skewtched a triangle onto the top face so that i can extrude out what i need from the block so the bit can sit in there.  my only problem is that since the bit itself is tapered, im trying to do the same as i negative extrude away the triangular shape from the solid block.  anyway, im stumped, and im hoping someone on here can shed some light onto my dilema, thanks in advance.  

[NicolasXu]

Hi Zerb,

Do you mean you want to add a taper for the extrusion? There is an option in the Extrude dialog to control the Taper Angle. Is it something you’re after?

Regards,

[Zerb]

I'm looking at the extrude dialog that pops up when I attempt to extrude the triangle into the block I have and all I can see is
Profile
Distance
Direction
Operation
Extents

Is that the dialog you're referring to? Or am I looking in the incorrect place?

But yes. That's what I'm looking for. In essence I want to take a cone and taper it into the flat surface of a block.

[NicolasXu]

Hi Zerb,

Thanks for the information. I understand the problem now. The Taper Angle option will appear only after we give a distance.

I will discuss with our UX and see how we can improve the experience. Thanks again for your feedback!

[Zerb]

The taper option I assume is the little blue ball looking thing that appears on screen that you are able to click and drag in a semi circle to alter the angle of the extrusion? Is that what you're referring to? Or am i missing something else all together.

If my above statement is correct. Is there no other way of getting a tapered object extruded into a solid object?

[NicolasXu]

Yes, we can use the little blue ball (we called manipulator) to alter the angle of the extrusion or type the angle in the dialog.

Depends on how complex the sketch profile is, we could also use other commands, like Draft, Loft, etc. to create the tapered object, but Extrude with taper angle would be the quickest way if the results can satisfy the design intent.

BTW, you may notice there is an Operation option is the Extrude dialog, it's to control if you want to cut (in this case) or create a new body. It's a common option in many Fusion commands to control the boolean result (join together, cut, intersection, etc.).

Hope it's clear. Please feel free to let us know if there is any more questions.

[Zerb]

I'll have to play around with it some more tomorrow. As I gave up for the night.

Say you take a 4x4 box, extrude it 1 inch upward. Then on that top face sketch a triangle. Now extrude that triangle, BUT at the tip of the triangle I only want to extrude about .125 inches into the cube, and at the bottom of the triangle I want to extrude .50 inches into the cube.

Does that better explain what I'm trying to accomplish?

[NicolasXu · Accepted solution]

Sorry, I misinterpreted the intent. Extrude with taper angle is not the right approach here, which will add the taper along the extrude direction.

If I understand it correctly, you want to create a semi-cone shape to hold the drill bits. I recorded a screencast to show how to use the Revolve command to cut the box.

If it’s not what you want (saying you want a flat side face?), could you attach some screenshots to show a similar shape so we can give more accurate suggestions?

Regards,

[NicolasXu]

I also recorded a screencast to show how to use the Combine command to cut the body, just in case you want to know the approach. In this case, the side and the bottom face are flat.

[Zerb]

That first video looks exactly like what I would like to do! Thanks so much. I'll try and give it a whirl later on tonight.

[Zerb]

Just did this and it worked out great!

My question is though you do Sketch Dimension on the one side of the bottom of the triangle, why only the one side and not the other as well? Also, what is the reason for adding the one line down the center? Is that so the Revolve function has something to go by? Lastly, the horizontal line near the tip of the triangle, then you went to symmetrical and selected both long sides of the triangle sketch, then to Sketch Dinension and selected one side of the triangle and then the center line and gave that a Dimension, why?

Sorry. I'm glad I can watch this and do it, but I'd like to learn as much as I can in regards to what I'm actually doing so I can apply that elsewhere later on if need be. Thanks!

[NicolasXu]

Hi Zerb,

Glad to hear it worked. Here are some answers for your questions. Please let me know if any unclear. 

When you do Sketch Dimension on the one side of the bottom of the triangle, why only the one side and not the other as well?

[Nicolas:] We have multiple ways to define the sketch. Because we want to use the Revolve command to cut the shape of the drill bits, the key here is to define the half of the section then revolve it around the axis. As shown in the screenshot below, the left one "could be" the exact profile of the half of the section. The right one is the section profile, but we only use the half for revolve. Also, in the previous screencast, I didn’t trim the sketch. All of the sketch profiles are OK in this case, as long as it contains the half of the section.

Also, what is the reason for adding the one line down the center? Is that so the Revolve function has something to go by?

[Nicolas] Yes, the line would be used as the axis for Revolve. It’s also the symmetrical line/center line of the section.

Lastly, the horizontal line near the tip of the triangle, then you went to symmetrical and selected both long sides of the triangle sketch, then to Sketch Dimension and selected one side of the triangle and then the center line and gave that a Dimension, why?

[Nicolas] Adding symmetrical constraint was just to make sure the triangle sketch is an isosceles one, so it can represent the section of the holder. The centerline/symmetrical line can divide the section into two halves.  

Regards,