It looks like SWX re-recognizes model's features each time and changes features ID's.
Delete mates. Create independent from features planes and use them to build a new mates.
It's a good practice to lock (using freeze bar) once all features is recognized so you don't have to worry anything weird happened in the future
Hai Christian thank you for your suggestion
I tried with your suggestion still iam facing the same issue
Is there any reason you want to use recognized feature to convert step file to SW? as we all know that you'd have issue soon or later? search on the group and there are many discussion about this topic?
I always accept the step file as it is and add any change if necessary - By the way, not sure if you're aware that you can insert the step file directly to SW assembly (available SW2017)
The reason is our vendor need to transfer all the project in SOLIDWORK format from inventor (They migrating from inventor to solidworks)
They need editable (Parametric models) models, It is easy to them to modify the parts easily in future, if it is non editable (Imported) it is very difficult to modify.
We have two option to convert the file to parametric from .Stp or .igs format.
1) Create the model from the scratch
2) With feature recognition option
First method take more time & complicate compare to second one because
we need to copy the sketch, check the relation between the sketches, check the hole wizard (Hole standard, size & type) & measure the dimension from the other cad software (it takes approx. 20 to 30 minute for a simple part)
But second one is very helpful, it is directly converted the sketches, holes, chamfer and other featutes as it is from the other cad software (it takes approx. 3 to 5 minute for same part)
we prefer second option because we have more than 500 files
I would say option 1 will save you the most time over the life of the project as you can already see the time you are spending trying to correct issues with option 2, because the issues with option 2 won't go away......
I just saw a response you made on another similar post - that you put a link back to this post. I had gotten way behind on looking at posts and didn't get back to seeing this one.
I do a lot of converting from Inventor to SW but I have never been able to convert an Inventor assembly to SW and have any mates remain. It may be that I am still on SW 2015 or maybe I am missing something.
I also found that the Inventor software has a much better conversion utility than the SW FeatureWorks to convert Inventor .iam or .prt files to SolidWorks files.
If you have the the Inventor program loaded on the same computer that has SW, you can just drag the .iam file (Inventor Assembly) from Windows explorer (with SW running)(Inventor NOT running) into the SW working area. (Don't have Featureworks set to open automatically). When the assembly file is dragged in, it will automatically open a "Inventor to Solidworks converter" utility (part of Inventor). It will ask you if you want to covert to Body or Features. Select Features. It will then automatically open every part in the assembly and convert it to a SW part, creating all the files and while it does this it will resolve all the features and create a feature tree - similar to what FeaturWorks will do but it does a much better job of recreating the design flow and features more the way you would actually create the part. It will do this automatically for each part, saving each part in it's own file. Much easier and faster and better results.
If you or your vendor has both programs it would be worth a try so see if this makes it better for you.
This doesn't address your question about the assembly mating, but since I am not on 2017 I can't test that and I suspect that is an improvement in SW since 2015 that allows the mating.
Hope this helps some.
What version of SolidWorks are you using (Year and type)?
When you import the step file and use Feature Works to recognize the individual features of the part what does the feature tree look like?
Does it look like a part you created from scratch or is it still showing just solids?
Can you post the feature tree for us to see - after you have run the feature recognition.
After you recognize the features, do you then save the part so that is saves as a xxx.sldprt file before you try using it in the assembly.
If you do not first save it as a SolidWorks part it may not save correctly or mate correctly to your assembly.
Then if you close the part and then re-open it again does it still look like it did with all the features showing in the feature tree?
I have converted many files of different types to SWX parts and converted them using FeaturWorks and never had a problem - even if FeatureWorks was not able to fully recognize all the individual parts (leaving some as dumb solids).
I have run into this before, I just tricked SW into the mates. I used Insert Face (+.010) on the features I needed to mate to, then cut them back to size but leaving .0001 so I had a 'new' feature in the tree.