Assembly Sketches and Mates to Sketches

marc_koeppel

I'm pretty new to OnShape and have just started trying it out, but I can't find a way to create a sketch in an assembly, and then I would want to mate to this path I have created.  I use this a lot to define a motion path for dynamic items, or robots.  Also is there not an assembly pattern as well.  I would put these items high on my list of needed features along with 2D drawings, and hole wizard (or feature library).  I assume all of this is in the pipeline, but are there expected release dates?  I have seen other forums on similar subjects, but expected release dates are not mentioned.  I would say that a product road map would be very helpful for those wanting to try out new features as they become available.  I would expect most users can't just be sitting around waiting and checking for updates.

_Ðave_

Dave_Petit is sitting around waiting and checking for updates.

andrew_troup

Given Onshape's unusual and highly responsive public beta development model, which involves massively parallel real-time bi-directional conduits with the testing public, I would not hold your breath for a roadmap: this is a much more organic model than we are used to seeing for industrial-strength solid modelling software.

I personally think it would not make sense to try to reproduce attributes of the radically different conventional model, because that would involve the risk of "falling between two stools" 

A very imperfect analogy would be of a country with a highly participatory democracy (binding referenda and such) deciding to publish a timeline for the passing of future legislation.

lougallo

Having a layout sketches is in the hopper for the ability to build skeleton sketches to drive assembly foundations is coming.  Obviously there are some workarounds with using a part for this but ultimately it is a workaround and we want to support the workflows that make sense.

_Ðave_

@lougallo Thx for the workaround tip. Yep its just a workaround but a clever one at that!

marc_koeppel

Andrew, I think you hit the nail on the head with the "industrial strength solid modelling software" statement.  People who are considering this software run businesses.  I can't go to an engineering manager and propose that this new software may be worth investigating when I have no idea when the features we need to make it viable for our business will be available.  I can see where this organic model works in the consumer products world, but for business this is a leap too far.

3dcad

Onshape is a bit weird betaware since usually all the features are there but there is a lot of bugs and other anomalies. I have only noticed very few bugs but I still understand that beta is for beta testing - it is not finished software for production use.

Of course Ons guys could keep all this behind closed doors and create all the functions and features without asking anything from anyone. But I think they have chosen a much much better way listening to people who are interested in their software at this early stage and already thinking / learning how to use Ons when it's ready.  

I remember few years ago when Alibre added a bunch of features with every update, then they had this voting system for new features and the most voted were: 'Fix all the bugs' and 'Usability before new features'. I'm glad they did.

I would rather wait 2 years for a significantly better product than having tomorrow just another cad. We already have a bunch of decent cad packages available so I don't understand what's the rush here (among us who are not working in Onshape). 

brucebartlett

I remember few years ago when Alibre added a bunch of features with every update, then they had this voting system for new features and the most voted were: 'Fix all the bugs' and 'Usability before new features'. I'm glad they did.

I would rather wait 2 years for a significantly better product than having tomorrow just another cad. We already have a bunch of decent cad packages available so I don't understand what's the rush here (among us who are not working in Onshape). 

@3dcad Onshape has been extremely stable and had very few bugs (none that have affected me) since I'v been using it. I have always thought that stability should come before fancy features, I think what Onshape have done by moving to the cloud is to be able to crete a platform for stability with the program running across multiple instances and I am sure this is still being tested as more and more users come on board and the features expand. The features will come on board and I am inpatient waiting for them, but I don't want fancy features, I want well thought out usable features that equal and even sometimes improve upon existing CAD without limiting the perform or stability.

When I am at my day job I am constantly running into problem areas; crashes, simple changes to an existing released product with out messing with the release models, or make a mistake and want to step back a few hours, etc, etc, and I find myself thinking Onshape will fix all these issues. But Onshape at this point in time could not possibly be implemented in this business, however given time and a full feature list and improved internet infrastructure we might see the move across.

traveler_hauptman

lougallo said:

Having a layout sketches is in the hopper for the ability to build skeleton sketches to drive assembly foundations is coming.  Obviously there are some workarounds with using a part for this but ultimately it is a workaround and we want to support the workflows that make sense.

Curves for motion are great but why is there a need for layout sketches? Aren't part studios in-context assemblies? Aren't sketches in part studios also layout sketches?

christopher_owens

@lougallo  @traveler_hauptman  Hello! I just ran across this too! I use to use a "Skeleton Part" in both Pro/E and SolidWorks that mostly had coordinate systems in it to quickly assemble components. Recreating my sports lighting structures reminded me of that! The individual steel tubes don't touch (until welded) so I was trying to figure out how to easily assemble them. Actually the "Transform-Copy" in Parts Studio (or Linear Pattern) would be handy in Assembly. Sure I can do that in Parts Studio and get the locations and "drop" those into an assembly and Fix, but the BOM would be incorrect. I'd have a Part 1<1>;Part 2<1>; Part 3<1> & Part 4<1> , when what I really want is a Part 1<1>;Part 1<2>;Part 2<1> & Part 2<2>. I have been "trying" to make Mate Connectors, but they need to be "in space" (like at the Origin/Default CSys of the part), or somehow creating a "Skeleton Part" that would have points or surfaces to use as mates. Still working on that one!

christopher_owens

Maybe I'll try the "Orb" I use to use in Pro/Cabling. The "Orb" contained the default planes, csys , xyz axis' and a point. I created a sphere just so I could see the thing! In Pro/Cabling you routed the wiring harnesses in an assembly, so I would place these "orbs" in space, route the harness through them, and them could drag to orbs around to reroute the harness. But in OS you can't see a sketch or datums in assembly yet...sooo...

christopher_owens

I have created a "Skeleton Part". Using a sketch with Points at locations that I determined are "Mate Connectors", and a simple Revolve sphere to make a Part (renamed Skeleton Part). I then use the points to create Mate Connectors and link them to the Skeleton Part.


I use the same points to create Mate Connectors linked to  the components. The first part in the assembly is the Skeleton Part which displays it's Mate Connectors...



Then I can bring in the other components...



Then I can Fastened Mate the component parts into place! I Fix the Skeleton Part in place at the Origin also.



Now my steel tubes that don't touch each other are in the proper locations and I can Hide the Skeleton Part to not see the "Orb"!



Thoughts @lougallo , @traveler_hauptman , &  @andrew_troup ?!

andrew_troup

3dcad said:

Onshape is a bit weird betaware since usually all the features are there but there is a lot of bugs and other anomalies. I have only noticed very few bugs but I still understand that beta is for beta testing - it is not finished software for production use.

Of course Ons guys could keep all this behind closed doors and create all the functions and features without asking anything from anyone. But I think they have chosen a much much better way listening to people who are interested in their software at this early stage and already thinking / learning how to use Ons when it's ready.  

I remember few years ago when Alibre added a bunch of features with every update, then they had this voting system for new features and the most voted were: 'Fix all the bugs' and 'Usability before new features'. I'm glad they did.

I would rather wait 2 years for a significantly better product than having tomorrow just another cad. We already have a bunch of decent cad packages available so I don't understand what's the rush here (among us who are not working in Onshape). 

Bravo: well said! (I missed this post when you wrote it) 

andrew_troup

@christopher_owens
Maybe it would be good to have some sort of streamlined input dialog (or other front end) for creating multiple mate connectors "in space"?

I suppose one challenge is capturing design intent. It's not at all future-proof, if it's just raw data, eg distances and angles

Another consideration: It seems to me (from my standpoint of relative ignorance) that one of the challenges of any sort of 3D input is being able to orient oneself in that space.
Occasionally someone comes up with something which really rocks. I recall Microstation nailed another aspect of this problem decades ago (possibly with something called "Intellisketch"?) - as a way of routing pipes, cables, ropes (around sheaves) - any 3D sketch involving alternating lines and tangent arcs at arbitrary angles.

traveler_hauptman

Take this with a grain of salt as I'm not 100% sure I understand your starting assumptions and goals.

I think you're trying a little too hard. I think one can keep the studio for top-down design and assemblies for BOM/sub-assemblies (ie actual manufacturing assemblies). 

For your simple example above, I would add part studio mate connectors at whatever nominal locations make sense.

I worked up an example with a couple approaches embedded. https://cad.onshape.com/documents/14820c8e9ed54f9a9dd4d5b7/w/bac1541a0c534a67b0234b2f/e/75382cd2c08342baa6330ba3

There's a lot of possible approaches. Here's what I did:

• My layout sketch captures the frame boundary and tube protrusion distance. Most likely you have some standard tube sizes and weldment process standards and capture the centerline instead. comme ci comme ça.
  
• Onshape automatic mate connect heuristics will locate the second moment of area of a face, so the end-face of the tubes need no manual mate connectors.
  
• "*complementary mate connector" uses the crossbar end face for location but is attached to the riser part. The allows the design sketch to drive the offset.
• Alternately "*Sketched mate connector" uses a sketch to put a manual mate connector at the center of a crossbar hole. The offset is entered manually.
  
• Group mates can join fixed parts whose location in the part studio matches the final assembly location.

There's more ways to do this. I believe they are fully generalizable. I started working up an example with imported off-the-shelf tubing, cut to fit the design sketch, but while it works fine it the feature tree organization and annotation capabilities of Onshape are so poor that it was difficult to follow so I switched to the simpler, more contrived example above.

The BOM problems created by using copy-part features in a part studio is a known problem discussed elsewhere. I'm pretty sure adding the ability to label/differentiate between copy->new_part and copy->new_instance is in their issues list.

Hope that helps.

christopher_owens

Everything helps! My example is of a unique design for one minor league ballpark. I next will reproduce the "family table" of cross arms that go from two lights up to 24 lights. Starting with one "short" main tube and a "short" cross arm (which vary in thickness), up to a "tall" main tube with three "long" cross arms. So the Skeleton Part would have all the Mate Connectors for these variations, and the main tube and cross arms would then be "family tables" of the various lengths. Again just trying to redo what I was "use to" in Pro/E and SolidWorks (and that worked!!) in Onshape. Basically the Mate Connectors would stay in place as the various parts "grow" around them. Ultimately we all do what works for us!

christopher_owens

From my past experience, the Default Csys in a part did not move or change size/angle. So it was a "safe" and quick way to assemble things. One assembly step and the part is "locked" in space and orientation. Plus you can place parts in the assemble in any order you want. Goes back to routing wiring harnesses all over LARGE pieces of construction/mining equipment and not want to "pull up" the whole machine to locate an electrical connector. So you get use to "floating" things in space. So when you do need to bring in an engine or frame it "looks" like things mate up, but all are "hanging in space" on coordinate systems. Plus you just put other peoples components on the "agreed upon" main csys's and everything lines up. Plus if another's part was modified or failed, my stuff didn't "unassemble", just kept hanging around.

christopher_owens

Hey! That URL address for an image really works slick!! My "trying to hard" is to end up assembling final structures easily. The above structure ends up here! Nice to know these a still hanging above the ball park!

_Ðave_

Nice Job Christopher_Owen! I Enjoy reading the daily adventures of Christopher_Owen on this Forum.
Keep up the gr8 work.

Dave

christopher_owens

LOL @da_vicki ! Yes I do tend to Comment as I think of things! But everything I have Commented about ends up being used in the "next adventure"! And don't forget the "s" on the end of "Owens"! One of my pet peeves! Cheers!

traveler_hauptman

@christopher_owens I get why you want the skeleton part in the assembly now. I can see how it speeds up the workflow and I would do it the same way.