Extrude from face

wcrisman

I would like the option to extrude a sketch from a face (object, surface) with our without an offset.

This is very handy when sketching something that is extruded in multiple places.  An example might be a fastener that occurs on both sides of a model.  I would like to sketch it once on one side, and extrude it on that side, then extrude it again on the other side of the model without recreating the sketch on the other side of the model.  

I do see how to extrude TO a model, but it seems like all extrudes in OnShape must start at the sketch.  Being able to start the extrude from other places along the sketch plane's normal would really be very useful.

MBartlett21

@wcrisman
You can use flip the second direction to have it act as a start face and use up to... on it

wcrisman

I have tried using the tools you mention without any success.  Flip simply switches the starting point of the extrusion to the other side of the sketch.  What I am asking for is that the start of the extrusion be at an offset (from another object and/or with a measured offset) instead of from the sketch.  This is a tool I have used a lot with Fusion.  I will create a sketch in any parallel plane, and then when extruding specify a start offset or surface in addition to an ending offset or surface. 

If OnShape supports this, it is so well hidden as to be useless.  A simple option to select a starting face or offset from the sketch (or selected face), similar to the UI that lets you select an ending face and/or offset is exactly what is needed.

Some background.  I teach CAD to JR/HS students and while I like Fusion a lot, it does not run on Chromebooks.  We have tried the education version of Sketchup, but it is not a parametric CAD, and it is too easy for the students to make a simple click error and have their drawing go wildly off the rails.  OnShape does run on Chromebooks and is thus a much better fit for teaching in a school that cannot afford special computer equipment for a single class.  Anything that makes OnShape easier to use (less repeating of actions in this case), makes it a lot easier to get the kids to believe they can do it.

romeograham

You can use the "Second End Position" check box. Set the directions the same, and make sure that your "second" position is closer to your sketch plane than your "blind".

You can use this with various combinations of directions and "offset" from faces - it becomes quite powerful (though figuring out the directions of the offsets is sometimes baffling).

Hope this helps.

wcrisman

I see now how you expect users to use this.

I would argue that this inverts the logic, making the UI more difficult to use. 

Instead of inverting the logic and removing parts of an extrusion you do not wish to have, wouldn't it be more straight forward to provide a start point?  

Ultimately it has the same effect, but from a UI standpoint the more direct logic is easier to use & comprehend.  From my standpoint teaching 7th graders and 9-12, the direct logic of a start and end point (versus an end point and removal of unwanted material), is a lot easier to teach to.

As evidence, I submit that I am a software engineer with 20+ years of experience, and this was difficult for me to figure out (I didn't without your help).

wcrisman

I ran into a more complicated situation while I was building a catapult for my lesson plan.  I designed a spring that is fixed to the axle and attached to the arm with a pin (so a coil with a hex center where it attaches to an axle, and a pin on the outside of the coil where it fits into the arm's hole - the spring is flush with the arm).  Extruding the first spring was simple as it was from the drawing flush with the arm, and then the pin that fits in the arm simply went the other direction.  The second spring was on the other side of the arm, so creating the spring from the same sketch as the first spring wasn't difficult using the inverted logic above.  Creating the pin was considerably more complicated since I needed to start the pin at the sketch, travel to the surface of the spring (to attach it to the spring), and then I needed to add a second direction, invert it, and then I could not figure out how to make it cut up to the spring's surface minus the 4mm the pin should stick out (I tried several things, but could not find a combination that worked).  Instead I had to hand measure the arm's width minus the 4mm, which means that if I ever change the arm's width, I will need to remember to recalculate the pin's width.

Honestly I can see a student (and most other people I have met in life) having a lot of trouble conceptualizing this, even if I could get the pin to be properly relative to the coil's position. 

Here is a link to the document in question.

Nem

Here is another workaround I've found if needing to use a surface/plane/face.

1. Extrude up to that entity (face/plane). 
2.Tick Offset distance box, tick reverse direction. This reverses the offset and makes the extrude feature extrude up from the plane or face in the same direction. 
3.Then use second end position to (reverse) back up to that face/plane, to remove any unwanted extrude.

The advantage of doing it this way means you are using the same face/plane as a reference, rather than Blind dimensions. Then if you need to move that face or plane it updates the extrude feature parametrically. 
I agree being able to select the face or plane and just extrude from that would be a good improvement, as it would be logical and intuitive.
Hope this helps too.


Ps. Putting in a negative offset distance value (-10mm), also does the same thing (but don't reverse the offset direction).

Also check out Lana's ( Onshape ) post on the same subject. 

romeograham

@Nem
This is a nice way to do it (using the Offset distance). It captures the design intent better....no second guessing.

wcrisman

That does the trick, but again I really think it is in everyone's best interest to add a UI for starting an extrusion (or cut) at a face or offset in order to make this straight forward logic (versus the inverted logic it currently is).

yurii_haiovyi

Yeah, it's confusing at best imo

NeilCooke

yurii_haiovyi said:

Yeah, it's confusing at best imo

That was so last year. Try it now.

Maurin

What would you do in the case of a multi plane pocket (see pic)?

I have had to symmetric revolve the cut from an elevation view sketch. extrude the hole bosses back. This is not exact because I had to calculate the degrees of revolve and revolve point, in order to get the correct "extrude remove" as Fusion does with an extrude FROM face, even if the face is multiplaned.

steve_shubin

@Maurin

It has been awhile since I did this

There might be a way it could be done with less features. But I don't have time to look at it now.

But for what it is worth, maybe this will help you.

The rendering was made from an export that I did out of Onshape and then imported into another program as I am not a PRO user and hence do not have the ability to use Onshape's rendering tools.

https://cad.onshape.com/documents/f9d1689d09a86fb4eec3225c/w/1f38e21ff4f4a4c9318415ed/e/522dd434ad63f47953f39f3e