Fixed Joint with tab in slot with clearance

[jlucasemail]

Trying to get a tab to fit into a rectangular opening with clearance.   I can get a corner to works and by adding an offset can get the clearance distributed evenly however, there are a lot each with different clearances so am hoping there is a simple way.  Easy to select centre of the tab but can't see how to select centre of the opening.

Thanks

[davebYYPCU]

Not checked the file yet.

If the hole in the purple block was done with a sketch, use the centre sketch point, to the centre of the green tab.

Might help....

[jhackney1972]

I would model the tab component complete and then assembly it with the hole component with any method you desire.  Afterwards use the Combine command to create the hole that matches the tab perfectly, no clearance.  Then use the Offset Face command to add the desired clearance easily to all sides or the ones you desire.  The Screencast will show the process.  Model is attached.

[jlucasemail]

Thanks, that's two excellent ideas.  In my case I have many objects to join and most will have been moved from their original positions so your ideas got me thinking (--dangerous--)

Fill the holes with separate bodies but part of the same component.  That way they move/copy with the frame.  Join to the center of these inserts.  Actually, only one hole needs to be filled for alignment, but if they are all filled and reduced by the clearance the inserts could be copied and combined as the tabs with the other components.

[davebYYPCU]

Bit backwards from where I am at.  If you have a complex problem, simple examples may not help.

Why make a 3rd item that is temporary and in my view unnecessary, when the proper sketching will do the same thing.

So I added centre points to the sketch, in two different ways, your choice.  Horizontal and Vertical constraint, or mid point constraint.  (Centre Point Rectangle it does it for you. 3rd option)

Setting joints to the centre point of each component is a simple set up.

Might help....

[jeff_strater]

to answer the specific question, you can use "between 2 faces" to do this.  See the screencast:

[g-andresen · Accepted solution]

Hi,

Here´s one more

günther

[jlucasemail]

Thanks guenther andresen but I don't see the alignment orientation menu.  Maybe because I am using t...

I have a master template sketch and build several bodies/components selecting various parts of the template.  When these components are moved into position the sketch is no longer available.  Did occur to me that I could build a sketch within each component projecting sufficient info for the alignment.  When moved the mini-sketch goes with the component.

If I can't get the alignment/reorientate menu I think the mini sketch is the best workaround.  Thanks everyone.

[jlucasemail]

Sorry, should read:  Maybe because I am using the student version?

[g-andresen]

Hi,

scroll or enlarge the menu

günther

[jlucasemail]

Sorry, no scroll or enlarge, its just a simple modal dialog box.   After selecting second snap point there is an alignment addition to the entry panel with angle, offset and flip.  None are helpful.

Says Windows 10 but actually 11.

[jhackney1972 · Accepted solution]

@g-andresen  is in the Joint Origin command, you are in the Joint command.

[jlucasemail]

Ah! Getting somewhere and can now orientate the 1st snap point but no way to select the second. Same type of model dialog without resize or scroll. Only option is save/cancel. If I save then the 1st snap point is still shown and I can now create a regular joint to it i.e. a 2 step process. If I edit the joint origin still cannot add the second snap point.

I'm accepting your response and closing this thread as I can now do what I want so thank you. Just confusing having to use 2 steps for this situation. Again, thanks.

[g-andresen]

Hi,

here are 2 more methods that work with only one Joint Origin:
1. measure offset and copy & paste.

2. invert component selection

günther