why does solidworks models and step files do not stay mated. I was told by my VAR that this was resolved SW2015 lied to again.
What exactly do you mean? A STEP file doesn't contain any mate information, and a SOLIDWORKS assembly will only have SOLIDWORKS parts in it. As such, I am really not sure what you are trying to accomplish.
If you can clarify your intent, I might be able to assist you.
i received a step file, piece part or an assembly. I saved it as a part. I add it to my solidworks assy, I mate it to SW created parts and attach SW created parts to it. Mate them all is good. Add this assembly to another assembly. mate it all is good. coincidence, concentric, distance limit,
come to these assemblies and all the mates are red, It does not matter the mate they all go bad. I need to go back and reattach them. Sometimes they stay, but mostly they keeping loosing the mates. after design is completed I need to fix all the parts attached to the former step file.
very frustrating when you need to move parts in the design process.
There may be different "options" you need to choose when opening the "step" file in SW. When you choose the file to open in SW there will be an "options" box in the lower left portion of the dialog box. Try different selections there to see if it makes any difference in how it acts. Also, be sure you are saving the step file as a SW file.
sw 2015 i do not get an option box when i open a step file
I am using SW2015. When I open a step file, there is an "options" box above the file type selection area.
Can you create and post a simple sample assy (complete with parts) to review what's happening?
it happened again,i do not know how to link the assembly, the step file is a slide from parker, i always have issues with slides from parker
I am guessing that you have native Solidworks files (built in Solidworks with features) and imported Soidworks files (imported step files) mated together in an assembly. Now you will get a new step file which is a later version of an existing file and you import it again with a new name (or the same name in a different folder). When you replace the existing mated imported file with the new imported one, likely all mates will become dangling.
Can you confirm that this is the issue?
When you open a step file, Solidworks imports the geometry and creates a Solidworks file with the imported geometry. Every geometric entity of a body has a specific ID and this ID is remembered i.e. in mates. Those IDs get created on import. Not sure what triggers the entity ID but usually those IDs do not match even though the imported geometry might be very similar. When the new ID does not match the remembered ID in the mate, the mate will become dangling.
When you know which faces will be used for mates, you can override the internal IDs with custom names (i.e. when you RMB on a face you can select "Face Properties" (you might have to expand the RMB menu since this option is not displayed by default) and then you can specify a name for this face). This custom name is remembered in the mate and when the new part has an identical face name the faces will be replaced without making the mates dangling (at least when the geometry allows the replacement; you definitely cannot replace a i.e. a cylindrical face with a planar face even though the names might match).
Hope this helps
Solidworks Product Definition Team
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