Width mate

kevin_shaw

In solidworks, I commonly use a Width mate to place a rectangular part equidistant between two faces.  I typically need this for fixtures that hold a PCB (Printed Circuit Board) and I want the board centered between the two interior faces of the fixture.  Is there something similar in OnShape.  I am exploring OnShape now.  I have looked at the Pin Slot mate, but it's just too specific for just one task. 

jakeramsley

If it is between two faces of the same part, you can move the mate connector into the middle with the 'Between entities' option.

1. I have two parts that I want to center one inside of the other in my assembly.  Because it is a rectangular hole, there is no implicit way to get the center of it.


2. I went to my assembly and inserted the grey part.  The first thing I did was start a mate connector on the middle of the edge in the direction I wanted.


3. Change the type from 'On entity' to 'Between entities'.  For the entity to be between, select the opposite face.  This will put the mate connector, aligned the way it was before, between the edge and the face.  This now gives me a point that is in the middle of the two faces.

john_christensen307

That's excellent for when it is between "two faces of the same part" but what about two faces of a different part.  For example.  I am working on aligning my battlebot wheels in the middle of my frame (multiple pieces).  I have shared my bot, Maximum Event with the support staff.

Armindilo

As noted, this doesn't work on faces of different parts. Is there a solution yet?

raj_Onshape

Armindilo said:

As noted, this doesn't work on faces of different parts. Is there a solution yet?

Can you share an example ? One can also offset mateconnectors to achieve the desired effect

Armindilo

ptrajkumar said:

Armindilo said:

As noted, this doesn't work on faces of different parts. Is there a solution yet?

Can you share an example ? One can also offset mateconnectors to achieve the desired effect

Offset would only work if the distance between the faces is constant, which it would not be of one of the items we on a slide or similar mate. 

I can't do an example right now, but just create an assembly with 3 parts and try to mate one equidistant between the other two, regardless of the distance between the two changes.

I'll model up an example later on tonight if needed.

3dcad

@Armindilo
Like this ?
https://cad.onshape.com/documents/d29ff8e74a0f49809e533f48/w/48fedb2064cc4f30a27ee6e8/e/c46b2fdb9683db1db3177334

Armindilo

3dcad said:

@Armindilo
Like this ?
https://cad.onshape.com/documents/d29ff8e74a0f49809e533f48/w/48fedb2064cc4f30a27ee6e8/e/c46b2fdb9683db1db3177334

Not really. That solution only works if the items are on Slider mates. If I want it to work on other arrangements where things are not always in line, and are free to move around in multiple directions, I end up having to add a lot of other mates to try to make it work properly, as well as having an opportunity for error if I don't calculate the original midpoint properly, since it seems to need to be set up manually. 

https://cad.onshape.com/documents/63edd3009dcfb0269fbaa894/w/cd6411299a5477651df1cc97/e/93ac2ff9499805d08a9512b9

nathan_gf

I also find the width mate very useful.  
In this example I mated the yellow block as I would like it.  But the pin slot mate only works because I added the blue part underneath.  The blue part also won't work if the walls need to be moved, unless it is defined in context to the assembly.
If I had wanted to center between the walls that would be a nice mate to be able to add.  

Another way might be to allow defining an assembly mate connector.  Then I could make a mate connector that is in the center of the two walls, and use a pin mate.

Another nice thing would be to be able to lock rotation within the one mate.  Either as part of the pin slot mate, or if there were a new mate for width.

Here is the assy
https://cad.onshape.com/documents/c626f606201f02555c041717/w/c2fe71c06476213040360097/e/a04fb84b13eaf7cddc410110

andrew_magaletti

I know this is a really old thread, but is there any solution to this yet? Being able to establish a mate connector directly between two parts would be very helpful.

matthew_stacy

@andrew_magaletti, the best I could come up with is a very crude work-around, by using a sketch to both mate the two parts together and then mate the third part to the midpoint of the sketch element.  The roller is centered between the two blocks shown below similar to a "width" mate in SolidWorks. 

Unfortunately you would have to edit the sketch at the Part Studio level to change the spacing between the blocks.

michael3424

Too bad that "Between Entities" doesn't work for 2 parts.

steve_shubin

andrew_magaletti said:

I know this is a really old thread, but is there any solution to this yet?

There is a at least a partial solution. But it takes some work

https://cad.onshape.com/documents/92972a0a94f295ddcf05858c/w/7eeddd97d49f27c00840448d/e/a5c7d7d0f201bbb6a9bec497

https://cad.onshape.com/documents/fe17150a8614096e96fcf21d/w/6d027c98f8ca54943f4b3f89/e/643c25206807ebf0d7911309

eric_pesty

You can do this using a linear mate relation like this no, or am I missing something?

I used two planar mates so the middle bit can move around up/down and sideways but you could make one of them a slider if you wanted them to stay aligned...



https://cad.onshape.com/documents/83a755253b5234cbf13ab537/w/61109c6b7dba48adaf5f9a77/e/c8a1bb398efd9186045c5af9?renderMode=0&uiState=61f044894799ad2097f82777

steve_shubin

@eric_pesty

eric_pesty said:

… or am I missing something?

https://cad.onshape.com/documents/e30a8944ef4fd87c73567eb4/w/e1590bba9447318544e0de2f/e/3e2f673abc952124a6cead71

No, you’re not missing anything. It was a great idea you had

I’m headed down to the basement to get the weed blower to blow the cobwebs out of my skull.

The relation let me do what I was trying to figure out yesterday

To be able to move the outside parts anywhere within a sphere

I would like to figure out how to not use as many mate features

I’ll go get a cup of coffee maybe that’ll help

eric_pesty

@steve_shubin
Moving along a sphere is a bit different from the original topic which was to replicate the Solidworks "Width" functionality which I think my earlier example achieves with two mates and a linear relation (not ideal but not a horrible workaround and doesn't need any "dummy" parts).

Looks like you can achieve something similar to what you are doing with 2 parallel mates (you can apply limit to rotation to keep them aligned) and 3 separate relations to link the x, y and z (and no dummy/helper parts):

https://cad.onshape.com/documents/83a755253b5234cbf13ab537/w/61109c6b7dba48adaf5f9a77/e/e261f52ba22643f6f6c16d46?renderMode=0&uiState=61f0af9cac0dfc508ff9e59f

steve_shubin

@eric_pesty

That’s excellent 

Do me a favor and unlock that thing so I can copy it. I wanna take a look at that

eric_pesty

@steve_shubin
Here you go, this should be public now instead of just a shared link: https://cad.onshape.com/documents/47c6c3f8282244773d012ab6/w/45c05cff81617055c12ed2f3/e/35595c8a9c42ad7502f40f26?renderMode=0&uiState=61f1867c27b84159870a69a5

steve_shubin

@eric_pesty

When setting up a linear relation on an iPhone, you will NOT see this menu

In other words, there’s no way to do what you did by using an iPhone. At least not anyway I could figure out, other than using dummy parts like I did above

So I had to fire up my MacBook Pro to get your combination of mate features to work

I definitely prefer your more lean approach

Thanks for that example Eric

eric_pesty

@steve_shubin
That's interesting about the limitation on Mobile.
It seems to that picking the degree of freedom is  a key part of creating a "mate relation" so I wonder if it's a bug (might as well disable mate relations altogether on mobile if you can't set them up properly...), you might want to fil a bug report...