I have come across a new problem.
When ever I make a new part in an assembly that has its first sketch on a a plane the part does not stay in its defined spot.
This never used to happen.
try to break the reference
Thanks for responding. I just uploaded some screen shots
Could you either upload your assembly or screen shots of what you're trying to do??
If I'm reading this right, the part is only defined by one plane....the one it's created on.
If I was doing this, I'd just fix the part. Either that or lock down the part origin in reference to the other parts.
at least show the mates of the part...
If you are creating a new part in the context of an assembly you should see an InPlace mate. This is what keeps the part from moving in the assembly. Your sketch being fully defined has no bearing on whether the part is fully defined in the assembly. I do not see the InPlace mate in your first image (see attached).
The InPlace mate is generated when you select a plane to initiate your new part on. If, however, you hit escape when SW is prompting for the plane, then the part is Fixed instead of being defined with the InPlace mate (see attached).
I am not sure where either your InPlace mate or your (f) Fix status went but this is why your part is not fully defined. Again, your sketches being fully defined will still allow your part to move within the assembly. Sketches not fully defined will allow features to move within your part regardless of whether the part is fully defined or not within the assembly.
You need to fully define your parts. Either (f) Fix them where they are - if you are CERTAIN they are in the proper location (not my recommendation). Or add new mates to locate them within the assembly. You can select the origins of your assembly and your part and add a coincident mate (with the Align Axes checked). Or you can add traditional mates that will fully define the part's location in the context of the assembly.
When creating a part in the context of an assembly, it is best practice to select the FRONT plane of the assembly when you initiate the part REGARDLESS of where you intend to sketch. This causes the part's planes to be in alignment with the assembly's planes. If you do not want to sketch on the front plane, cancel out of the auto-launched sketch and proceed to sketch how / where your design intent directs. But it is important to first select the front plane (aligns to assembly and creates the InPlace mate).
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