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I'm trying to use a width mate to make sure the spherical protrusions in the pin are equal lengths away from the selected ends of the body.
Can someone explain this to me in a step by step process?
Categories: Modeling and Assemblies, Assemblies
Let me know if you need the model files for better reference.
You need planer faces to do width mate. Try using a center plane on the pin and doing a symmetric mate.
On the left side of the screen select advanced mates, pick width mate. From there you have to select 2 faces on the mating part and 2 faces on the mated part.
Im not sure it will work on spherical faces, I may be wrong.
There is 2 boxes on the width mate, the first is for your component which would be the pin, select the two features you want the width about, the next box is the component you want to be centered on you select the two features you want to be centered between.
Lowell,.. this will not work on the spherical ends unless you apply a small flat on each end?... or, if you added a radius at the ends of the cylinder pin (say it's dia 2mm).. make the radii R0.99 and use the flats at the ends.
...otherwise, use a symmetry mate, .. the center plane of the pin.
In addition to what Paul said,,, you could probably add planes at the base of each dome on the pin and do your "width mate" using those planes. Most of the time I would use the symmetry mate assuming I have a plane already existing in the center of the pin.
This is what I actually did, but the problem was that it wasn't fixed in: when I clicked the part it moved. Is that supposed to happen?
Thank you all for the swift responses!
If you have a symmetry mate or width mate and the concentric for the hole, the only movement should be rotational.
Did the mate get added? (If it is the most recent mate, it should be at the bottom of the mates folder.)
I would've tried what you said and given feedback, but unfortunately one of the parts just went missing, so I'll remake it and post feedback soon.
Edit: I did the concentric mate and width mate, but the width mate wasn't at the bottom, when I had both parts.
Edit: It still keeps translating and rotating. The planes are on the base of the hemispherical bodies.
How would I use the symmetry mate for this? I put a plane in the middle.
What happens if you "fix" your latch, or make it coincident with the right plane?
(Does the pin move separately from the latch, or are they moving together?)
The pin moves separately from the latch but concentrically, so it stays within the holes. The latch is fixed.
No Lowell,, that not supposed to happen. It would still be able to rotate on the concentric mate unless you lock rotation. It appears you have added the planes in the assembly and not the part environment. You need to edit the part and add the planes at the part level.
This is what the mate in the tree should look like.
Ah that worked! Thanks!
Thank you to everyone who chimed in!
Just want to chime in with a little note. If you hole your CTRL button while selecting the 4 planer surfaces an icon for the width mate will appear under the heads up display. You can select that and you don't need to go into the mate menu. This works for any type of mate you want to create. Hold the CTRL, select the surfaces and all available mates will pop up. However I have found that if your last selection is on the upper or to the right portion of the screen the Icons don't always show up.
Coolest thing about this method is that you DO NOT need to select them in any particular order!