Add vs New Extruded Part for Subtraction etc

william_holden959

Even though I've had an account, I'm finally diving-in (recently from Solidworks). So, I'm new.... I really need the part studio top-down design concept and am liking the concept. I need two cylindrical parts that connect on the edges that provide an adjustable gap between them when you turn one against the other. The profile of the edge has to have "steps" so they can't slide out of adjustment. I'm just trying to make a matching part and do a subtraction. Any help/advice is appreciated. (On a different note, it'd be nice if there was a multi-segmented helix. No need to get degrees or clockwise vs counterclockwise, just pick a point on an existing helix to add pitch and turn. And maybe be able to add filets to the profile?)

https://cad.onshape.com/documents/7ad64ad01976b9fb8b394990/w/c1ded4c1c3a49011d881d699/e/c5426a8ed6f39451e759b186

Jake_Rosenfeld

@william_holden

You need to change your extrude to "Solid" rather than "Surface", and use "New".  Then in the boolean, you can do "Subtraction" with the blue part as the "tool" and the grey part as the "target", making sure to select "keep tools" so that the grey part is not consumed.

Jake_Rosenfeld

You also may want to not use "Offset all" in favor of just offsetting the top faces that you care about offsetting (otherwise the side faces are offset as well and the geometry is odd.)

I copied your document and made the changes as described

https://cad.onshape.com/documents/2be35d16a23f6d4eab635755/w/53059868b6705c634fdeebd4/e/60a5a69a43a57025ef8d7d3f

Jake_Rosenfeld

@william_holden959

The face will not be selectable in "surface" mode, It will only be selectable in "solid" mode.  If you pre-select the face and then press the Extrude button, it will automatically be in "solid" mode, but I suspect you got into "surface" mode by pre-selecting the edge and then pressing the Extrude button.

Additionally, if the face is not there at all to select, you may have to "show" the sketch by clicking the eye next to the sketch feature in the feature list (It will only show up if you hover your mouse over the sketch feature), and you may have to hide certain parts (eye button in the parts list) to get at the sketch once it is shown.

To select the offset faces I had to "hide" part 2 temporarily (while the feature dialog was still being edited), select all the top step faces, and then show part 2 again

MBartlett21

william_holden959 said:

On another tangent (figurative), it appears that I can't do an extrude/cut beginning at an offset distance.

You can.
You can add a second direction and click the opposite direction button for it.

Jake_Rosenfeld

@william_holden959 @MBartlett21

Oh how dense I am!  I'm actually the one who implemented extrue-up-to-with-offset and then failed to realize it was the right solution for this case...

I've created a version in the same document, and made some edits to reflect the better way!
(In addition to what M. said, I've also backed the plane up an additional 4mm so that the extrude only needs one end position instead of two.  Extruding with offset has a quirky behavior that if the offset pushes the faces through to the other side of the profile, the extrude will fail )


https://cad.onshape.com/documents/2be35d16a23f6d4eab635755/w/53059868b6705c634fdeebd4/e/60a5a69a43a57025ef8d7d3f

Jake_Rosenfeld

@william_holden

You need to change your extrude to "Solid" rather than "Surface", and use "New".  Then in the boolean, you can do "Subtraction" with the blue part as the "tool" and the grey part as the "target", making sure to select "keep tools" so that the grey part is not consumed.

Jake_Rosenfeld

You also may want to not use "Offset all" in favor of just offsetting the top faces that you care about offsetting (otherwise the side faces are offset as well and the geometry is odd.)

I copied your document and made the changes as described

https://cad.onshape.com/documents/2be35d16a23f6d4eab635755/w/53059868b6705c634fdeebd4/e/60a5a69a43a57025ef8d7d3f

william_holden959

Thanks Jake! I swear I tried all that! Not sure why it was surface and not solid. The faces that you have selected for the offset are not showing up for me (I'm not able to select those). But, you got me heading in the right direction. This is the way I understood it to work, not sure what I missed before somehow getting "surface"

Jake_Rosenfeld

@william_holden959

The face will not be selectable in "surface" mode, It will only be selectable in "solid" mode.  If you pre-select the face and then press the Extrude button, it will automatically be in "solid" mode, but I suspect you got into "surface" mode by pre-selecting the edge and then pressing the Extrude button.

Additionally, if the face is not there at all to select, you may have to "show" the sketch by clicking the eye next to the sketch feature in the feature list (It will only show up if you hover your mouse over the sketch feature), and you may have to hide certain parts (eye button in the parts list) to get at the sketch once it is shown.

To select the offset faces I had to "hide" part 2 temporarily (while the feature dialog was still being edited), select all the top step faces, and then show part 2 again

william_holden959

OK! Suppressing the 2nd Part and picking each surface for the offset was what I was missing. I'm not sure why that would be necessary. It seems like I should be able to pick the large surface on the back of the part as long as I give it a relative distance. On another tangent (figurative), it appears that I can't do an extrude/cut beginning at an offset distance. But, I realize I have not gotten deep into this and I appreciate everything this offers. And thanks again for your help!

MBartlett21

william_holden959 said:

On another tangent (figurative), it appears that I can't do an extrude/cut beginning at an offset distance.

You can.
You can add a second direction and click the opposite direction button for it.

Jake_Rosenfeld

@william_holden959 @MBartlett21

Oh how dense I am!  I'm actually the one who implemented extrue-up-to-with-offset and then failed to realize it was the right solution for this case...

I've created a version in the same document, and made some edits to reflect the better way!
(In addition to what M. said, I've also backed the plane up an additional 4mm so that the extrude only needs one end position instead of two.  Extruding with offset has a quirky behavior that if the offset pushes the faces through to the other side of the profile, the extrude will fail )


https://cad.onshape.com/documents/2be35d16a23f6d4eab635755/w/53059868b6705c634fdeebd4/e/60a5a69a43a57025ef8d7d3f

william_holden959

If you want to have a dense-off, I'll win every time! I'll take a look at it. What I ended-up doing is not using the offset at all, because in the assembly I can set it up the way I need. But I want to understand it, so I'll look- but no promises that I'll be able to get my mind around it.

I have to say that I am incredibly happy with what Onshape offers. I've checked it out over the years, and I am blown away. It is exactly what I need. Thanks for the help!

william_holden959

That's an excellent feature!! Great Stuff! I was able to include that. Now I'm redoing the part and this particular type of extrude isn't working for me. It might have to do with new circular pattern that I'm extruding to. When I made the circular pattern, it gave me a little trouble, so I'm a little suspicious. The failed extrude is the last feature. Thanks for all the help!

Jake_Rosenfeld

@william_holden959

Feel free to post that document link here also if you want someone to take a look I thought you may be referring to your original doc, but I don't see a circular pattern or a failing extrude.

william_holden959

@Jake_Rosenfeld I was trying to extrude to the part while it had a hole through it. So, it was my fault and I figured it out after I posted the comment. It's a very power feature! I appreciate all the behind-the-scenes work going on!