Extrude From (Starting Position)

adrian_vlzkz

According to the closing of this IR, there is no need for the "Extrude From" or starting position in Onshape, but I have a scenario that I think proves different.

Closed IR:
https://forum.onshape.com/discussion/comment/35060#Comment_35060

NeilCooke

Totally agree - an option to offset the "extrude from" plane would be very useful and if the IR is closed I would open a new one. The way to do this now is to use a mate connector as your sketch plane and edit the mate connector to add an offset - if the master sketch is shared with other features then you would have to create a new sketch and "use" the edge.

adrian_vlzkz

Thanks Neil, two of our designers pointed this out the first day they started using Onshape (transitioning from SWx) so I would say is much necessary.

EvanReese

Other issues with the current solution are that it takes phenomenally more clicks and knowhow to do than just picking a plane, and the extruded parts still draft from the sketch plane, and there's no way around it with the current implementation. I'd love a starting entity query.

billy2

The new way works fine and is more flexible & sensible.

It's best to drag the handles into approximate locations:


Then attach to geometry:


This is the preferred way to do it. 


Please leave solidworks behind and learn onshape.

adrian_vlzkz

@billy2, not complaining about the current method in Onshape, just asking for extended capability to meet our design needs.  Your example assumes the same as why they closed the IR, does not capture the intent.

 And we are trying to leave SWx that's why we are asking for this missing use case.

S1mon

It's nice to know that I can get some of the "from vertex" "to vertex" functionality that I'm used to from Solidworks.

However, the current system doesn't let me model in draft the way that I've been doing it in Solidworks. I use a ton of extrude from vertex with draft. The draft hinges from the plane which is parallel to the sketch plane that contains the vertex. In Onshape the draft hinges from the sketch plane regardless of the other settings. I like to sketch a lot on the default planes and only create other planes when I absolutely have to (lofts etc). The Onshape way forces me to create extra planes or mate connectors and/or draft features.

Other things missing (compared with Solidworks):

• no draft option on an extruded surface
• no option to extrude along a vector other than normal to the sketch

NeilCooke

Draft extruded surface can be achieved with Ruled Surface 

billy2

@adrian_vlzkz it's good to see you get these guys moving into the future.

I had a lot of issues with this feature in the beginning and Lou Gallo said that it had a lot of attention from focus groups to develop. He asked me to give it a chance. After about a month of playing with it, it started to sink in.

Maybe this could help, have both "up to face" reference the same face and then offset the furthest giving you the distance offset you're wanting, you don't have to compute it.




One thing to remember is the 1st end position has to be further away from the sketch than the 2nd end position.

Keep pushing them & good luck! If you need some help, let me know.

S1mon

NeilCooke said:

Draft extruded surface can be achieved with Ruled Surface 

Using Ruled Surface accomplishes a lot of what one might want to do with an extruded and drafted surface. It's a decent work around. However, there are no options for extrusion depth or up to a surface or body (let alone offsets from these). The distance parameter of a ruled surface is not the same as the depth parameter of an extrusion.

billy2

@S1mon drafted surfaces would be nice. I just add it as a 2nd draft feature.

I haven't played with ruled surfaces yet and want to. It was a missing puzzle piece and I'm glad it was added.

Since this thread is turning into a surface want list, how about extrude curve in this direction, and, let's add draft to that.

I'm not sure we'll ever stop wanting things, OS surfacing is pretty good these days.

S1mon

billy2 said:

@S1mon Since this thread is turning into a surface want list, how about extrude curve in this direction, and, let's add draft to that.

Extruding in a direction with draft is essentially possible with Ruled Surface, but it just doesn't have the depth options of Extrude.

adrian_vlzkz

billy2 said:

@adrian_vlzkz it's good to see you get these guys moving into the future.

I had a lot of issues with this feature in the beginning and Lou Gallo said that it had a lot of attention from focus groups to develop. He asked me to give it a chance. After about a month of playing with it, it started to sink in.

Maybe this could help, have both "up to face" reference the same face and then offset the furthest giving you the distance offset you're wanting, you don't have to compute it.




One thing to remember is the 1st end position has to be further away from the sketch than the 2nd end position.

Keep pushing them & good luck! If you need some help, let me know.

This method doesn't provide a way to enter the desired thickness of the extrude. You have to make the calculations manually or create more ref geometry.

edward_petrillo

I'm not modelling for a living, and I hardly ever encounter surfaces or drafts.  I've settled into a workflow where all of my geometry is defined in sketches on the native planes, and all of my extrudes are "up to vertex" and "up to vertex" (same or opposite direction).  No "magic numbers" (numerical values) in my feature dialogues, so I can read all of the relevant dimensions in the sketches.  I avoid "up to face"  because maybe that face will disappear down the line.  The result is I'm opening and editing the sketches more often than the features.  One exception:  "up to part"  can be very useful in certain situations.  

If I ever dipped my toe into Featurescript, the first thing I'd probably write is a stripped-down Extrude with nothing but inputs for the sketch regions and the two vertices.  That would save me lots of mouse clicks!

S1mon

edward_petrillo said:

I'm not modelling for a living, and I hardly ever encounter surfaces or drafts.  I've settled into a workflow where all of my geometry is defined in sketches on the native planes, and all of my extrudes are "up to vertex" and "up to vertex" (same or opposite direction).  No "magic numbers" (numerical values) in my feature dialogues, so I can read all of the relevant dimensions in the sketches.  I avoid "up to face"  because maybe that face will disappear down the line.  The result is I'm opening and editing the sketches more often than the features.  One exception:  "up to part"  can be very useful in certain situations.  

I'm glad I'm not the only one that likes working this way. Since a sketch is solved all at once, it's really easy to go into the sketch and change a dimensioning scheme, whereas a plane offset from a plane offset from a plane is a recipe for disaster.

S1mon

So here's some interesting behavior... you can extrude multiple sketches at once in the same extrude feature. The sketches do not have to be coplanar, and don't even have to be on a parallel plane. They do extrude in the direction of the first sketch. This adds some interesting possibilities to do extrudes in a direction without it being normal to a sketch. In the screenshot, Extrude 2 is using Sketch 2 and Sketch 3, but all the material is being added in the direction normal to Sketch 2. The circle sketched on the chamfer is producing an elliptical cross-section protrusion.

billy2

@adrian_vlzkz I think this is the same behavior that SW has, although there are more picks.

I want a 10mm  hole at a location specified face of rev1:


10mm entered and 10mm shown:

billy2

@S1mon that is interesting, I'm trying to figure out how to put that to use.

billy2

I got a chance to play with ruled surfaces this weekend and really like them. After loft, ruled surfaces are my tool of choice and I've been wanting them since the beginning of OS.

Here's a simple example of ruled surfaces:

* I have a non-planar parting line where the part needs to be split for 2 mold halves
* 7 features and 1 cleanup feature
* it's extremely robust and creates a well formed manifold



Then someone comes along and wants to make a changes:

* they change the size, curvatures & thickness
* can your model handle changes?



The simple anatomy using ruled surfaces:

* it starts with a surface shape containing compound curvatures
* then you create ruled surfaces for the top & bottom
* then you fill the top & bottom
* then I added a loft to form cleaner outer curvature



Surfaces used to create manifold:

* this manifold contains no slivers, shortened edges and gives you a clean part that can be used for downstream manufacturing
* some surfaces are just scaffolding for other surfaces which is typical for surface modeling, you build surfaces to create surfaces
* you can control complex shapes and capture design intent that'll speed development due to a clean b-rep manifold



The most important step:

This model is driven from a compound curvature surface and in this model it's declared as a datum stating that it's driving everything in this model. Datums don't have to be flat planes in parametric solid models. I think I'm mixing up forum threads, sorry, datums are important. 

Having worked on 100's of injection modeled designs, this complex datum is always missing. To recreate it from trimmed faces is almost impossible and you never know if you have it right. All translations can give you solids and surfaces. Please include this datum in your dataset for the next guy.

Also, if you're creating injection molded parts, use surfaces. Even if it's for datum definitions only, your models will be clearer and better formed. Pushing geometry to their extremes in a solid model only creates sliver surfaces and issues making the geometry un-usable for subsequent manufacturing operations.

billy2

@adrian_vlzkz probably the simplest way to move past this issue, it's quite simple, it's easy and it's available now.

Have @Evan_Reese write you a feature script that does exactly what you need. That's what feature script does and as good as Evan is, he could write it less time than we've spent creating this post.

EvanReese

billy2 said:

@adrian_vlzkz probably the simplest way to move past this issue, it's quite simple, it's easy and it's available now.

Have @Evan_Reese write you a feature script that does exactly what you need. That's what feature script does and as good as Evan is, he could write it less time than we've spent creating this post.

Haha, thanks @billy2. Flattering but probably false. I bet @Alex_Kempen could though.

Alex_Kempen

I've been summoned! Funnily enough, I do have a FeatureScript capable of doing exactly what @adrian_vlzkz has described - it's called Plate extrude, and it's part of my larger suite of FeatureScripts aimed at optimizing the creation of 2D plates. Notably, Plate extrude lets you choose the start plane of your extrude irrespective of the defining sketch plane, and it also has useful options like symmetric up to and they ability to extrude separately (which extrudes each face as a new part, even if it touches other extruded faces).
You can find plate extrude and my other plate suite features here:
https://cad.onshape.com/documents/2c2b49357f3f1a232881256a/w/6258e1943ecedc8606542dd7/e/78e9b9148efe7163309beca0

billy2

@Alex_Kempen amazing, that didn't take long. 

Brad_Goodman

I'm trying to follow this ridiculously long and complex thread, for a simple feature which I think everyone agrees is really a fundamental thing that should be added to avoid some very cumbersome and frequently-needed workarounds.

Anyone know if there was an IR added, or this is being considered for inclusion??

adrian_vlzkz

Just wanted to chime-in, given the most recent update. Do it is a great step forward, it still does not fully address the original use case I presented.

There's still no direct way to "offset from face", specifying a distance. The only way I was able to create the desired scenario was to create a Mate Connector within the extrude feature. The issues with this is that the parameters for that mate connector are hidden within the Start offset Entity.

Yes the end-result is achievable, but my original request was not about end-result, was about the steps required to do so, and intuitive would be communicate design intent.