Why did you guys make the mates suck again?

Why don't use the component preview window when mating?

The mates work just fine for me with SW17-SP1, no different than before.

So before, I was able to select two planes on two parts and the planes would align and nothing else.

Can you explain what you mean by this? What else is happening for you now?

Now when I do the same thing the two parts move really close together and I have to manually move then again just to make another mate. 

If you are aligning planes why wouldn't you expect the parts to move closer together?
Why would you have to move the parts to make another mate?

If you don't want the parts to move till all the mates have been applied, deselect the Show preview option in the Mates Manager.

It's a 'sticky' option so you only have to do it once.

Matthew,

I'm pretty sure the new behavior that Dennis described is causing you the heartache, but I assume you know that you can click and drag components while the Mate command is active?  That will help give a little more room between them to choose surfaces if they're placed too close.  (A 3d mouse is also a big help for rotating and zooming in and out.)

If you want a concentric and a coincident mate you can often achieve both by just selecting the two faces and selecting Profile mate.

I know you have your options posted, but checking or un-checking this - does it make a difference??

select Edge- Alt-drag, will give you concentric and coincident at the same time.

But you probably need space for a Gasket.

I've been experiencing the same problem. I was directed to this thread and the only way I can now do it is to turn the mate preview off, select the faces to be mated and then turn the preview back on. The component only moves to satisfy that mate.

It's a nice feature for me sometimes but given the option I'd probably turn it off and leave it off.

I feel your pain, and understand the issue you're asking about. I'm a plant\manufacturing engineer, so I use SW for everything from mechanical assemblies to facilities. In either of those cases though, unless it's a concentric assembly (i.e. - round objects), I typically follow the same pattern of initial placement. I almost always insert the first component by mating the assembly and part origins and build everything from there. The next component I insert is typically in free space, but when I start to constrain it, say starting with a coincident mate, it moves the floating object to the mouse click point that I chose on the fixed object. Often, if the floating part is smaller, and I pick say well within the fixed part, it places the coincident mate, but by moving the floating part to that mouse click point (instead of simply truing it up out in space) it winds up within the fixed part. Since I can't select the part because it's "hidden" within another part, I have to select it from the tree, go to "Move Component", throw it out in space, and then continue on with my mate commands. It never did this prior to 2017, or at least SP 2.0.

Two ways maybe they could address this to make everyone happy: either give us a radio button to cut this off, or make it smart: if I have a fixed part and a floating part, and I initiate a coincident between the two, if it's going to move the floating part within some proximity to the fixed part, sense that we're dealing with two solids, and prevent them from occupying the same space (this seems to me the most intelligent fix, but if not, give the option to turn it off, because it's causing a lot more work).

Hi Matthew,

We're sorry that the new functionality isn't working for you.  Whilst we have addressed a couple of issues that resulted in behaviour that wasn't intended, having seen your workflow, it's clear that you'd like to be able to turn this off.

Would a system option be suitable?

Thanks,
Chris

I'm surprised nobody has mentioned Select Other. When the parts move close to each other there is no need to move them farther apart, or rotate to pick the inner faces. Just Select Other and dig down to get the faces you want. That's the fastest way for me.

Mate Reference can help as well.  I do not believe I saw it mentioned yet but they work great when you use standard parts over and over.  You create a Mate Reference with the same name in both parts using the mates as you need them (i.e. Concentric, distance, coincident, etc.).  Then when you drag the second part in it will snap to the first part like a toolbox hardware part does.  Full Defined for you with no extra work.  It may not be best for all situations but it should work for most.

Steve

sometimes it worth changing the settings via a macro. I know it sounds a bit crazy but I've had issues with some of the settings that got resolved when I used macros to change them.

Try changing the magnetic mate proximity with its enumeration. It should have solved the issue when you did it in the settings yourself but give the macro a try too.

Hi Matt, I think I may have something for you. In your part create an offset surface (3/32") or what ever. Then create 2 mate references. One concentric (diameter on part) and one coincident (surface). Now do the same for the mating part, but no surface . (make sure there named the same thing on both components). Now tile the windows vertically (assembly and part) and drag part into assembly close to mating part. It should snap into place. (you can toggle orientation with tab key). Surface does not add any weight and can be hidden. You could even add a tertiary ref to orient (clock) component.