Powerful workarounds

andrew_troup

It is likely to be some time before Onshape's Revolve command will feature advanced end conditions like "up to vertex".
I'm not even sure that Solidworks has it yet.

There's a relatively simple workaround available now: If you set up a sketch arc*, you can use it as a path to sweep the 'revolve' profile along.
The resulting geometry is analytical, and as pure as that of a revolve.

* on a plane normal to the revolve axis, ending at the desired vertex.
NOTE: it is not widely realised that the arc (or any sweep path) does not need to be anywhere near the profile being swept (or revolved, if you prefer)

This exact capability is not something which many people will end up needing, but I think it illustrates the value of striving for a fundamental understanding of what the various tools can achieve.

If you can avoid a mindset where the limitations or even absence of a particular command seem like showstoppers -- the classic "glass being half empty", a lot can be done with the fact that it is simultaneously half full. 

Extruding at an angle is another task, on the face of it not possible in Onshape, which is actually very straightforward using a sweep. Again, the path can be remote from the profile.

andrew_troup

Someone else recently pointed out, on this forum, that the "up to vertex" end condition (similarly not yet available in Onshape) can also be simulated for an extrude, using a sweep in a similar fashion to the previous post, but with a straight line for the path.

If the line is angled rather than normal to the sketch plane, this is a workaround for the SW "extrude at angle"

andrew_troup

In the interests of collecting a number of workarounds into a compact resource, a handful more:

Project sketch to a sketch (to produce a 3D curve): extrude the sketches as surfaces, choosing for the second extrude the end condition "up to surface". The terminal edge of the second surface will be the desired curve.
This is currently mainly useful for sweep paths, and can even be used for such things as variable diameter helices.

To derive a sketch into the same part studio: Copy the sketch into a dedicated part studio (if there are several, you could call it something like "Master Parts") then derive the sketch back into the original studio (it would probably pay to replace the original sketch as well, so all similar sketches shared a common parent). If necessary, use "Transform" to move it into position. (Courtesy of @philip_thomas)

To achieve the same effect as simple equations (using arithmetic or simple trig) use a dedicated sketch to carry out the operations graphically. Use the "Equal" constraint to move data into and out of the processing diagrams

To simulate a reference axis, create a dedicated sketch on a suitably defined plane with a constrained line, and leave it visible.

To simulate "Cut with Surface": use a surface to split a part, then delete the unwanted portion (thanks @abefeldman).

For radial text: refer https://forum.onshape.com/discussion/1346/any-work-around-method-to-insert-radial-text-in-sketch

To copy a part from one document to another: copy the whole part studio, then delete the unwanted parts.

To reinstate an isolated operation (not including subsequent ops) from History: refer https://forum.onshape.com/discussion/1132/do-you-really-want-to-delete-this-parts-studio-tab-hope-your-sure

To insert labelled milestones or landmarks in the Feature List of a long Part Studio: refer "Defined Parts" tab of this model from @traveler_hauptman :  
https://cad.onshape.com/documents/3c4e14158ece451f8d1c7318/w/6e4e129fbdab428da966d8a4/e/88e72be15478404f8307f3cd

and for a simple way to delineate individual parts when built sequentially: Name the first feature of each new part in CAPITALS. (suggested by @da_vicki)

And the most powerful of all: the famous "Sketch Picture" workaround: https://forum.onshape.com/discussion/504/found-a-workaround-for-sketch-picture-feature   (note the posting date)

kevin_quigley

I missed that Sketch Picture thing! Brilliant, if a little mad! Alternatively, now, just do it in any number of paid or free graphics apps that allow dwg or dxf  export...

andrew_troup

There's a nifty demonstration by @philip_thomas showing how to simulate motion in a part studio for the purposes of in-context design, in the specific case where certain positions need to be captured in the conformation of other parts. It starts about 20m into this video clip:
https://www.onshape.com/videos/twio-multi-part

There's a cunning workaround within it which might have broader applicability: to make multiple (more than two) "Copies in place" of a part, he uses Linear Pattern with a distance of zero.
These copies are then moved to the desired locations using "Transform", and the incontext features created using those relocated parts.
Naturally a dedicated Part Studio can be used for this manipulation, especially now that we have "Derive Part"

3dcad

I'd like to add another workaround to have 'production drawings' without using drawings.

Tip 1.
If you have dimensions that are needed for sketch but are redundant for production you can create a copy of sketch and add only the dimensions that you need. Then exit sketch and use 'show dimensions' to get nice image.

Tip 2.
For imported models you can quickly add dimension sketch with 'Use/Project' tool. Add needed dimensions --> exit --> show dimensions.

Which one do you prefer:

andrew_troup

Here's a crafty stopgap for the current inability to rotate a sketch, courtesy of @shashank_aarya

https://us.v-cdn.net/5022071/uploads/editor/9k/pa841tr26ro1.gif

andrew_troup

Here's a barrel cam workaround supporting polar coordinates, to permit ad-hoc "wrapping" of a 2D path around a cylinder: 

https://cad.onshape.com/documents/23ea467e79014d19b4097729/w/942d64b50cdb4baf9889844e/e/6ae350e800ce47ec916a098a

The joint lines could be eliminated (or an assymetrical groove modelled) by making the first loft a closed one, wrapping the full turn, rather than my kludged half turn

ON EDIT: This "surface loft thru horizontal lines" method would also work to provide both a path and a horizontal parting surface for ball track toys, something recently requested on this forum

andrew_troup

andrew_troup said:

........

 the "up to vertex" end condition .... can be simulated for an extrude, using a sweep .... with a straight line for the path.
.......

Probably bad etiquette to quote myself, but what the hey!

Here's another approach which (in some cases) might be a more useful workaround :

A "Plane point" plane is like the end face of a (large) sketch extruded as a solid from the given plane, if you had chosen the given point as the end condition for an "up to vertex" extrusion.

So, as a workaround the current lack of that particular end condition, you could define a plane that way, before performing an extrude.

3dcad

I think @billy had good workaround using surfaces instead of planes since they are easier to create in various positions.

andrew_troup

3dcad said:

I think @billy had good workaround using surfaces instead of planes since they are easier to create in various positions.

Indeed he did !
I, too, thought it was excellent - and now I've learned the easy way to post a link to a specific message, here goes:
https://forum.onshape.com/discussion/comment/12267/#Comment_12267

andrew_troup

A slow and dirty workaround for (currently unavailable) configuring features, which could still be a very useful stop-gap until we get the real thing, kindly posted by @ilya_baran :

https://forum.onshape.com/discussion/comment/12690/#Comment_12690

andrew_troup

Regarding the configuration workaround: It's not quite as slow, and certainly not as dirty, in reality as in the imagination. 

Scroll down that same thread for a wonderful animated gif  @lougallo just posted, showing a simple but potent application of  Ilya's suggested method.

I reckon it wins hands down in living up to the description of the title of this thread.

BTW: Anyone else with decent workarounds is welcome to submit them directly here, or PM me first if you think they might not be fully worked out and want a second opinion.

andrew_troup

Another recent and interesting workaround from @ilya_baran was for conics. Here's how it looks for a parabola.

In the first graphic, the highlighted line is the axis of the revolved cone, which is then "Split" by a plane parallel to the generator line for that cone.


Here the highlighted line is the sweep path, which enables the parabolic edge to be turned into a surface, which can be used directly (eg by thickening), or as a tool (to split another body, or extrude up to, or a bunch of other possibilities)


I learned a couple of things:

1) An edge can be"extruded" as a surface (without first being converted to a sketch), using the workaround further up this thread, of substituting a sweep for an extrude.

2) A sweep path (if it uses a sketch line) cannot be a construction line.

andrew_troup

To create a planar (flat) spiral (Archimedean): 

https://forum.onshape.com/discussion/comment/12830/#Comment_12830

andrew_troup

To check for breaks in a chain of entities:

https://forum.onshape.com/discussion/comment/13281/#Comment_13281

andrew_troup

To work around the current absence of Assembly Planes: the Origin has an integral Mate connector

(Thanks, @matthew_menard  !)
https://forum.onshape.com/discussion/comment/13367/#Comment_13367