Note: an updated version of this post can be found here.
I recently ran into these weird mates in SolidWorks when I was using virtual parts. Then suddenly, the mates stopped appearing, and I blamed the computer for that. As usual, this wasn’t a piece of software acting inconsistently, it once again was a user action that triggered the change in behavior. I couldn’t find much info about the InPlace mates online, so I decided to document it myself.
What are InPlace mates?
InPlace mates are a special kind of Coincident mates that are only created when you work in an assembly with virtual parts. They mate a virtual part in all directions to an existing part, without fixing the parts in space. They are created automatically without any input from the user. You also can’t edit them, they can only be deleted. That’s why I see them as a placeholder, they exist until you replace them with proper mates.
When do they appear?
InPlace mates get created when you apply the following steps:
- Open an assembly
- Create a new virtual part by clicking Insert Components > New part. This will add a virtual part
- Select a plane that you want to start your first sketch on
- Have the No External References button disabled (so you can create external references)
- Create a sketch,
- Exit the Sketch mode
- Exit the Edit Component mode to back to the assembly
How can I keep them from appearing?
When you don’t want InPlace mates to be created, there is only one step that you have to do different. You have to enable the button No External References, shown in the image above. Once this option is enabled, you can no longer create relations to other parts in a sketch. This means there is no longer a need for an InPlace mate, so it will not be added. When you create your first sketch in a new virtual part and go back to the assembly, you’ll see that the part now remains mateless.
Did this post help you, did I make a mistake or do you have an idea on how to improve this post? Please let me know in the comments or shoot me an email.