Using Mates to Attach Radius to Flat Face

Logan_5

I am having difficulty using the mates in Onshape.  This doesn't seem uncommon for users coming from other CAD systems.  What's easy to do in another system seems more difficult to do in OS.

What's difficult to do is mate the rounded corners of the side plate to the flat face of the blank.  This is a very common case for my line of design work.  The side plates contact the blank face at the rounded corners labelled 1 & 2.  I was able to replicate this but not correctly by using the vertex at the beginning of the radius and use a tangent mate to attach it to the face. When I used the tangent mate and clicked the arc of the radius and the face of the blank the side plate became parallel to the blank.  This was not the desired result when I tried the vertex of the radius and the face.

The side plates are actually flared a little bit as you can see in the images below labelled Gap.  Typically I need to create a dimension for the offset at label 3.  This is another problem I am having trying to replicate this in OS.

Also, when I am pulling parts from another part studio into an assembly, I need to mirror the parts in the assembly so the BOM will be accurate.  How do you create a mirror in OS Assemblies?  As you can see in SW there are two side plates but only one in OS.

Can anyone help me replicate my SW results in OS?  If I were to switch to OS and this situation was not do-able, I would not be ablet to migrate over to OS.


Grey parts created in SolidWorks--Blue Parts created in Onshape (Side View)



Grey parts created in SolidWorks--Blue Parts created in Onshape (Front View)


https://cad.onshape.com/documents/79f6f2d9bce0c2e9d083f0bf/w/3c1abd814c3db4d0b27e2703/e/814f95e15860a1c1d226af75

Thanks,
Logan

Alex_Kempen

Constraining in Onshape works best when there is some point of flat contact between two parts. For example, constraining a screw into a hole is really easy because the flat head is centered on the round hole. There also isn't really a way to mirror parts in assemblies; instead, you should mirror the part in the part studio first. If the part isn't chiral, however, then you don't really have any options besides getting it into the proper location using assembly mates.

Of course, one easy way to circumvent these issues is to design the parts in the correct location relative to each other. Not only does this make designing the parts easier since you can see and reference the other part while designing, it also greatly simplifies assembly since inserting parts into the default position and then grouping them together constrains them robustly and quickly.

dirk_van_der_vaart

Maybe this is a simple solution, rotate around an axle.
https://cad.onshape.com/documents/e7e991f1acd531d7bc109fe5/w/71dd27b43c18dacb286564ce/e/addac5bd676745ad6795582f

tim_hess427

@Logan_5 - Its hard to tell how you have the positions defined in solidworks, so its difficult to say exactly how this should be done in onshape. 

One thing you might try is creating a sketch with key geometry/offsets and adding that to your assembly so that you can define the correct angles between your parts. How do you define the angle of the "flare"? What axis is that angle rotated around? 

Also - you can easily add multiples of any part into an assembly, by clicking on it more than once in the insert dialog. You can also click on a part in the assembly parts list and copy/paste to create another instance of it. 

Logan_5

This scenario has many different variations with a variety of side plate designs.  The option to design the parts in the position they should be in just can't happen.  If the ability to apply a tangent mate to the rounded edge was functional like SW then this wouldn't be an issue.

With regards to Assembly mirror not being a thing.  I can insert more instances but then recreating those tricky tangent mates becomes double the hassle and really a horrible experience with OS.  I wish the mates could utilize OS creative methods but also utilize the tried and true versions that most CAD systems use to help the transition. 

tim_hess427

@Logan_5 - I understand that those two highlighted edges need to be tangent to the middle part. But, what I'm not understanding is how do you define the position of those edges and the angle of the plate? From your screenshot, it looks like its sort of arbitrarily placed.

I'm asking because it may be possible to use a simple "fixed" mate with the right offsets and adjustments. Then, depending on how the mates are set up, you could probably leverage part studio and assembly configurations to create your variety of designs.

tim_hess427

To show you what I'm thinking - I made a couple edits to your linked assembly.

I added sketches to the side plate with lines that are tangent to the two edges labeled (1) and (2). I repeated this on both sides of the side plate. Then, I added a sketch with a line on your middle plate.

Now, you can add the sketches to the assembly (I used group mates to keep them with their owner parts), then used a quick "fasten mate" to connect mate the sketch lines together. Use the offset option on the mate to adjust the rotation angle around the z-axis of the mate.

https://cad.onshape.com/documents/97225c908a26d941f0c5a64b/w/2c21cbfc4e15329b23c3521a/e/9f2f6b79313a3e79e46bee00

Logan_5

tim_hess427 said:

To show you what I'm thinking - I made a couple edits to your linked assembly.

I added sketches to the side plate with lines that are tangent to the two edges labeled (1) and (2). I repeated this on both sides of the side plate. Then, I added a sketch with a line on your middle plate.

Now, you can add the sketches to the assembly (I used group mates to keep them with their owner parts), then used a quick "fasten mate" to connect mate the sketch lines together. Use the offset option on the mate to adjust the rotation angle around the z-axis of the mate.

https://cad.onshape.com/documents/97225c908a26d941f0c5a64b/w/2c21cbfc4e15329b23c3521a/e/9f2f6b79313a3e79e46bee00

Thanks, @tim_hess427 for the feedback.  I was curious and thought about adding the sketches as well.  It sort of works.  I normally set an offset dimension of 1/8" to 1/4" from the side-view perspective depending on which side plate I am using.  For this side plate I use 1/8" offset.



I tried a fastened mate between the two sketches and applied a rotation angle about the Z axis of 5 degrees.  It flared one side as expected but made the other side flat against the middle shank.  I have not had any luck getting the 1/8" offset to work.  Everything I do flattens the side plate against the blank.

Logan_5

This shouldn't be this hard to mate two objects together and then mirror it about a central part/plane.  I've had to create two extra sketches and import extra sketches into the assembly just to attempt to accomplish what I need to do, with no success yet. Onshape, please make mirroring parts in assemblies a thing and improve mates just a little more for odd applications like this.

I looked and could not find a plane reference in the Assembly.  Are planes not important for Assemblies?  Rhetorical question, yes of course they are.  Why aren't they here, Onshape?

tim_hess427

@Logan_5 - if you need a plane, you can just add a single mate connector wherever you need it (at the origin, or offset wherever you want it). They essentially act like a coordinate system and can be used as reference planes.

Logan_5

tim_hess427 said:

@Logan_5 - if you need a plane, you can just add a single mate connector wherever you need it (at the origin, or offset wherever you want it). They essentially act like a coordinate system and can be used as reference planes.

Thanks, @tim_hess427 I will give that a try in the next day or so.  I am just struggling with how to mate these odd-shaped parts together that aren't created in a part studio that references its final location.  I can't design it that way because each one would have a different angle between the side plates and the blank because of what goes between them.  Typically there would be a tube or something else that goes between the two side plates in the assembly that requires the side plates to be flared at different angles.

I have about 30 different side plates that we use for different applications on a couple of shank designs.  I thought the best way to organize the parts were to create a part studio with all the different side plates in it as flat patterns that we buy from a laser shop and then for each knife design have it be a separate part studio that I can import the side plates into the assembly and place them where I need them (similar to how I manage assemblies in SW).

@NeilCooke, can you assist or point me towards someone that can work with me directly to try and find a solution to this issue?

tim_hess427

@Logan_5 - if the angle is actually defined by the two tangent points along with a tube (or other part), why not include that tube or part in the assembly? 

Also, if you have 30 different side plate designs, splitting them into separate documents will allow you to more easily have version and revision control over them independently. 

Logan_5

tim_hess427 said:

@Logan_5 - if the angle is actually defined by the two tangent points along with a tube (or other part), why not include that tube or part in the assembly? 

Also, if you have 30 different side plate designs, splitting them into separate documents will allow you to more easily have version and revision control over them independently. 

@tim_hess427, I did not include the tube and other parts to keep things simple and proprietary information out of my public account.  I planned to create all the different kinds (shapes) of side plates in one document but make them in different part studios.  Is that what you mean by separate documents.  I should be able to do version control on the separate designs in separate part studios, correct?

tim_hess427

"Versions" are created at the document level while "revisions" apply to specific parts. So, even if you have the parts in different part studios, if the part studios are in the same document, they'll all be at the same "version" level. 

So, if you have a document with parts A, B, and C in separate part studios. You can create version 1 of that document. Then, insert part A-v1 into an assembly. You could then go back and modify part B and create version 2 of the document.  Over in your assembly, part A will show that there's an update available because the document was updated. 

However, once you release a part and create revision, then you can tell your assembly to only flag you if Part A is updated to a new revision level. 

This is one area where onshape is a little confusing, but can be powerful once you get a hang of it. 

Summary: "Versions" are snapshots of an entire document at a specific instance in time. "Revisions" apply to released parts and are tied to a specific part number.