Mate connectors in Part Studio stay behind when I transform their owner part

chris_8

Am I missing a way to bind the part to the mate connector?

thanks,
Chris



Example:
https://cad.onshape.com/documents/6b714e18e39e7a82c583e9db/w/1b919740fcf6075f60128924/e/3e3023a32957b2f261920b77

brucebartlett

Mate connectors don't bind to the part in the part studio but if you select the mate connector in the move feature it will move as well. 

brucebartlett

No, it is not possible to move a sketch with the move feature.

The only way to move a sketch would be by rolling before the sketch feature in the tree and move the sketch plane before the creation of the sketch. Off course this will also depend on how the sketch constraints are referenced to the origin or other geometry. 

brucebartlett

chris_8 said:

Now that I've cleaned up my Part Studio by including the mate connectors in the transform commands, those mate connectors can no longer be hidden.  Mate connectors that remained static can be hidden, but the ones that relocated are permanently visible it seems.

That's a bug, they should be able to be hidden. I'd report it with you feedback tool "?" top right.

philip_thomas

Ok, so i had a go at this, and it is a perfect storm.

Normally, a user would have at least one of the following;
1) Access to the part feature history - this would enable you to put the mate connector at the center of the bottom face before cutting away the cylindrical opening.
2) Two vertical faces that would allow you to use the 'between entities' option in the mate connector dialog.
3) The ability to derive in a mate connector attached to a part

In the absence of these, a sketch is the way to go.

chris_8

owen_sparks said:

I believe that if you hide the transform feature in your feature tree then that will hide the mate connector. 

Owen S.

I didn't even remotely consider that, but it works!

philip_thomas

@chris_8 - YES, you are correct.

'Between' enables you to position and orient a Mate Connector and then say 'but half way between this face and this one'
(this is straight from the help - https://cad.onshape.com/help/Content/mateconnector.htm)

brucebartlett

Mate connectors don't bind to the part in the part studio but if you select the mate connector in the move feature it will move as well. 

chris_8

brucebartlett said:

Mate connectors don't bind to the part in the part studio but if you select the mate connector in the move feature it will move as well. 

Thanks Bruce.  That works.   I realized there is an extra layer in my issue.  My example blocks were designed without all the features of the part studio that had sparked my question.  There was a sketch involved in my design, and the mate connector was attached to a midpoint on the sketch.  I had tried clicking on the sketch to have it moved as well, but it wouldn't get selected.   I didn't ever click on the mate connector itself until you mentioned it,  I think I had tunnel vision focusing on that sketch (see below). 

Now I know how to move the mate connector.  Is it possible to move the sketch as well?

https://cad.onshape.com/documents/6b714e18e39e7a82c583e9db/w/1b919740fcf6075f60128924/e/7fe629eee1ac35df8f394160


 

brucebartlett

No, it is not possible to move a sketch with the move feature.

The only way to move a sketch would be by rolling before the sketch feature in the tree and move the sketch plane before the creation of the sketch. Off course this will also depend on how the sketch constraints are referenced to the origin or other geometry. 

chris_8

Now that I've cleaned up my Part Studio by including the mate connectors in the transform commands, those mate connectors can no longer be hidden.  Mate connectors that remained static can be hidden, but the ones that relocated are permanently visible it seems.

brucebartlett

chris_8 said:

Now that I've cleaned up my Part Studio by including the mate connectors in the transform commands, those mate connectors can no longer be hidden.  Mate connectors that remained static can be hidden, but the ones that relocated are permanently visible it seems.

That's a bug, they should be able to be hidden. I'd report it with you feedback tool "?" top right.

chris_8

brucebartlett said:

That's a bug, they should be able to be hidden. I'd report it with you feedback tool "?" top right.

Done.  Have a great week

owen_sparks

I believe that if you hide the transform feature in your feature tree then that will hide the mate connector. 

Owen S.

philip_thomas

Ok, so i had a go at this, and it is a perfect storm.

Normally, a user would have at least one of the following;
1) Access to the part feature history - this would enable you to put the mate connector at the center of the bottom face before cutting away the cylindrical opening.
2) Two vertical faces that would allow you to use the 'between entities' option in the mate connector dialog.
3) The ability to derive in a mate connector attached to a part

In the absence of these, a sketch is the way to go.

chris_8

owen_sparks said:

I believe that if you hide the transform feature in your feature tree then that will hide the mate connector. 

Owen S.

I didn't even remotely consider that, but it works!

chris_8

philip_thomas said:

Ok, so i had a go at this, and it is a perfect storm.

Normally, a user would have at least one of the following;
1) Access to the part feature history - this would enable you to put the mate connector at the center of the bottom face before cutting away the cylindrical opening.
2) Two vertical faces that would allow you to use the 'between entities' option in the mate connector dialog.
3) The ability to derive in a mate connector attached to a part

In the absence of these, a sketch is the way to go.

1) This was a Mcmaster part import, so you're right: there was no access to a feature tree.

2) Honestly I didn't understand "Between entities" then.  I thought of entity as a body, but it can indicate 2 different faces from the same body?   That's good to know!

philip_thomas

@chris_8 - YES, you are correct.

'Between' enables you to position and orient a Mate Connector and then say 'but half way between this face and this one'
(this is straight from the help - https://cad.onshape.com/help/Content/mateconnector.htm)

chris_8

philip_thomas said:

@chris_8 - YES, you are correct.

'Between' enables you to position and orient a Mate Connector and then say 'but half way between this face and this one'
(this is straight from the help - https://cad.onshape.com/help/Content/mateconnector.htm)

I've been through that help before and I skirted around it because it didn't seem to work as I expected.  I didn't have a need for "between entities" at the time so I shrugged and moved on. 

After working with it this evening I realize my issue was misinterpreting the "between entity" box.  I expected to be able to specify 2 things in the "origin entity" box, and then expected the mate connector to appear in between the two.  But I could only choose 1 entity.  I saw the "between entity" box and thought I don't need to click there because I already chose Between entities.   

If entity 1 is an origin, I'd expect entity 2 to be a terminal or something.  Between is what I expect to happen between entity 1 and entity 2.  How does entity 2 get defined as between entity?

I get easily tripped up be wording in OS sometimes.  I went off on a rant about 'derived' years ago once I finally figured out what it's really for.  I'd been searching through help for Copy part, or Insert Copied Part, or Duplicate Part to no avail.  It Derived me crazy  

Now I know.  Thanks

owen_sparks

I agree the between entities feature input dialogue is slightly counter-intuitive.  I was expecting to pick two points not a point an a face, however once understood I like it a lot. 

In the example It's especially useful if you have some tolerance (slop from side to side) in the pin, so you don't want to mate a surface on one end of the pin to one side of the bracket.

Cheers,

Owen S.

MBartlett21

philip_thomas said:

@chris_8 - YES, you are correct.

'Between' enables you to position and orient a Mate Connector and then say 'but half way between this face and this one'
(this is straight from the help - https://cad.onshape.com/help/Content/mateconnector.htm)

@philip_thomas
I'd like to select a point as the between entity. Is there any way to do this?

philip_thomas

@mbartlett21 - you mean like this?



https://cad.onshape.com/documents/dfaa5483ff7746bf49404630/w/593df3a65236749750bc8614/e/a2695c0099131730ccd2801c

PeterM

Has anyone filed an improvement request on any of these issues? I think  mate connectors should move with the derived part in part studios when you transform the derived part. I see no reason for them to stay in the original location. And you should be able to hide them.

philip_thomas

@PMS - you are welcome to submit any enhancement request (and as a pro user we take them very seriously), but just to be clear, you can move the MC with the part(s) being transformed (just include the connector in the selection of things to move) - it's second nature to me now, but i just wanted to make sure you knew this - works great!