Extrude at an angle..not the right tool?

[nkloski]

I am trying to create some small features at an intersection of a flat plane and a block on top of that plane.  If everything were at 90 degrees, it would be trivial, but here is my issue:

As you can see, one edge is NOT at 90 degrees.....so here is what happens.  If I create a sketch on the back plane, that sketch is 2 degrees off when I try to extrude:

If I try to sweep the profile, I also get an error (plus the sweep command is not useful, since I cannot sweep in units (5mm, etc.), I can only deep in percentages of the path.  The error is below:

If I try to create a plane at an angle, then that would work, but then that plane overlaps empty space, which causes the above overhang problem in reverse:

All I am trying to do is extrude that profile a few millimeters to make a little wall, but that angle is getting in the way.  I guess I 'could' create multiple profiles and loft between them, but that seems like a lot of work for something that should be easier.

Anyone have any ideas?  Fusion file attached.

Thanks!

[etfrench]

Two extrudes and a delete face will get you where you want to go

First extrude to create the thickness of the wall.

Select the end of the wall and extrude it with the To Object option. 

This will leave a small face still extending past the desired end. Select and delete it.

[nkloski]

Thanks!  I did think of that but it bugs me to rely on the delete faces command.  That would work here, but it is not the best parametric way to do it.  That will help me in this case, but I have had other projects where multiple delete faces become hard to manage 😞

[etfrench]

You could also have just selected the bottom of the overhang and used Extrude|Cut to remove it.

[TheCADWhisperer]

---

@nkloskiwrote:

... not the best parametric way to do it.  

---

Something like this?  

[nkloski]

Ah, interesting!  Using the extrude/intersection to make the extrusion....that does work for this case, but it still seems like not the right tool for more complex shapes.  I will likely choose this as the answer, but I am still looking for a more straightforward way of extruding at an angle.  It may be that I have to use lofts to retain the parametricity, but that has much mroe overhead to do it that way.

[TrippyLighting]

You can simply use "split body" and "remove" that piece.

[nkloski]

Yep, that would work as well...but if there was a larger assembly in play, that would also be something that might make things more complex.  I just wish there was an extrude on rails command, that would be nice.....but I guess that is called a loft (though with more work to set up).

[StephenCim-001]

Would be nice if you could select a direction with the extrude ?

[nkloski]

Not sure what you mean?  You can choose between "forwards and back"....but I am looking for a more magical command that says "extrude a profile down this arbitrary line".  But again, that can be done with a loft, so I am more leaning to just having "hey you, use a loft with rails, you!"  be the answer 🙂

[TrippyLighting]

You can also use a sweep with guide rail (with the stretch option) but it will create different geometry.

And, of course you'd have to create another sketch if you use sweep if you want to define the sweep distance in mm, or inch.

[chrisplyler · Accepted solution]

---

@nkloskiwrote:

....but I am looking for a more magical command that says "extrude a profile down this arbitrary line".

---

There is a magic command for that. It's called Sweep.

If you want to sweep 5mm exactly, create a path that's 5mm long exactly.

[TheCADWhisperer]

---

@TrippyLightingwrote:

You can also use a sweep with guide rail (with the stretch option) but it will create different geometry. 

---

 Lost me there?  The Design Intent was already stated.  How does a solution that "creates different geometry" solve the Design Intent?

---

@chrisplylerwrote:

There is a magic command for that. It's called Sweep. 

---

Can someone post one of these "Magical Sweep" solutions for this particular geometry?

[TheCADWhisperer]

---

@nkloskiwrote:

Yep, that would work as well...but if ....

---

Post any file you have and I will attempt to discover a more efficient technique.

[TrippyLighting]

See attached.

[TheCADWhisperer]

---

@TrippyLightingwrote:

See attached.

---

I guess I didn't understand the original Design Intent statement - both of your planes are compound angles?

The OP will have to confirm the true Design Intent.

Did, or did not, my Extrude-Intersect honor the true Design Intent?

[TrippyLighting]

@TheCADWhisperer Your solution creates the same geometry as the non-sweep / split-body solution I posted above. Just by different means, but perfectly valid IMHO.

You are correct that, this can only be verified by the OP.

[nkloski]

Thanks, everyone!  I really appreciate everyone's responses!

I do not mean to offend, so one one take it that way but:  I am reticent to adopt a workflow that "affects the whole model"...like the Extrude/Intersect or the "Split Body" techniques would.  Those are inherently making "total area" changes to the model when all I want to affect is the one place I want to affect.

If it is true that those are the only workflows, then so be it, that's great.   I had a problem starting out when using the sweep command, as it introduced some errors I talked about in the original post of hidden/mismatched geometry.  But now when I try it again, I am unable to reproduce that sweep error.  Thanks everyone for the help!

[TrippyLighting]

---

@nkloski wrote:

...  Those are inherently making "toal area" changes to the model when all I want to affect is the one place I want to affect.

---

You can split a body locally with a face, if you don't want to split it with a plane. In that case you'll have to create a sketch and then a patch so you have actual geometry.

[nkloski]

Ah, interesting!  Using Patch as a scalpel tool, great tip!