I have a simple assmbly and few parts there. All cylindrical parts have same Mate Reference, but when I replace one of these parts with another, mate references doesn't work! What am I doing wrong here?
If you are using the replace component functionality, mate references don't work that way. Mate references allow you to insert parts and have it snap to the desired mating scheme. For dropping pins in, you will have better luck selecting the edge between the shaft and the head as the only reference, when you drop it in you will automatically get the concentric and coincident mates. The way you have them is intuitively what you think you would want, it just doesn't work that way reliably.
Reference only "Datums" in the mates for the parts you are wanting to be able to replace.
The "Mate References" you've created are simply for "auto-mating" components as you drag them in...not updating the mate references when you do a replace component.
I found mate references to be the most useful when building design libraries. I built a standard pipe straight, and added configurations for different pipe sizes (1/2" npt, 3/4" npt, 1" npt, etc...). I added planes that were offset from the ends and named the dimensions. I put together a design table and then changed the distances for each configuration based on effective thread engagement.
I set up the mate references coincident and anti-aligned to those planes, and concentric to the pipe. I kept the mate reference name the same ("Default"). The name is important as anything you want to mate to those references has to have the same name (that way the mating part will only mate to a mate reference of the same name).
For the fittings, I just made configurations for the various sizes and set up mate references to a PLANE coincident to the end of the face and concentric to an axis I created (cylindrical portion of the fitting).
Afterwards I just dragged and dropped fittings and built plumbing assemblies quickly. If I needed different sizes (for different skid plumbing sizes, but everything stays in the same location) then I just made a configuration within the assembly and changed the sizes of everything within the assembly--viola, everything adjusts accordingly. However, since different size pipe have different thread engagement I had to adjust the lengths of each pipe segment. This works much better if the pipe segments are virtual so you could modify everything without having to check anything out (if you're using EPDM).
I've done this for building wireways as well. Keep the individual components virtual so they could be modified easily. If I needed to remove a section then I'd delete a section assembly and drag in a new section and it would snap in place.
Long story short, they're very useful for things that have known parts/features. Don't work well if you're constantly designing something new. Make planes and axis and set those as the primary/secondary/tertiary reference entities that way when you replace the component the planes and axis are picked up instead of faces/features.
You'll have to troubleshoot it quite a bit if you want it to work correctly. Play with the "aligned", "anti-aligned", "any" settings to see what gives you best results. Make sure that the primary reference on one piece matches the primary reference on another...otherwise you'll have issues. Make sure the reference names are the same or you'll have issues.
One other trick is to press the "tab" key while a mating component is snapped (but don't place it yet), and it will switch alignments.
Okay, thank you all for good replys! I have not understood this right! Thought that it would help replacing components when automating some tasks. But need to find another way to handle mates when replacing components.
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