I use the same distance mate of .016" repeatedly to build a tolerance in for my CNC frames. I can't seem to find a way to change the default 1.000" to my standard tolerance. Is this possible, and if so, how do I do it? I would love to be able to select two faces and the distance mate and not have to manually input my tolerance every time. Thanks!
I'm not aware of any way to do it. I thought maybe a global variable would work, but it looks like Distance mates are one of those functions where they haven't yet gotten around to giving us the ability to insert equations directly.
Here are a few things to try:
1) If you are constantly using .016" in your assembly, then first create a global variable of .016". Then just add the distance mates at the default values. Then later, come back and open your equation manager and select "Dimension View".
Now, all your distance mates are right there. and you can change them on the fly.
Done.
OR
2) Change your length spin box increment to .016".
Then, once you are inside your mate command click in the distance mate and then hold down your down arrow key until it drops to 0. Then tap the up arrow key once. Now you are at .016. Not really faster....just easier on the typing fingers.
OR
3) Did you know that if you select your two surfaces (or whatever you want mated), then a pop up will appear. Select distance, and it is whatever the current distance is.
I will try the global variable option like both you and Glen have mentioned. I already have the spin box increment changed to the thickness of my extruded panel stock, so I don't want to change that. The pop up dialog box and regular dialog input box are where I am constantly typing currently.
Another thing that you can do is to add a reference plan inside your part (not inside your assembly) that is .016" from whatever you want mated. Then use a coincident mate in your assembly on that plane instead of a distance mate.
I'm sad to say, but adding a global variable isn't the right option for my workflow. Tried it, and have to change the equation manager every time before I can add in a new component. Adding in the reference plane has me still keying in the tolerance to define the plane. I feel like I am missing something big here. Maybe I change the spin box increment back to .016" and set up a custom material that is my normal stock thickness??
BTW, thanks for taking the time to help out. It is much appreciated.
Worth Berry wrote:
Tried it, and have to change the equation manager every time before I can add in a new component.
I am not sure that I understand this statement. Can you elaborate? Why do you have to do it before you add a new component?
I am building each part in my assembly off of the previous part and in relation to the whole assembly. When I let the default value define my distance mate, I have to immediately go in and change that mate to my "Nominal" value before I can build the next part in my frame. Is this any more clear?
Worth Berry wrote:
I am building each part in my assembly off of the previous part and in relation to the whole assembly. When I let the default value define my distance mate, I have to immediately go in and change that mate to my "Nominal" value before I can build the next part in my frame. Is this any more clear?
Ahh, well what I meant was to leave the default distance and let the frame assembly go extra large until you have all the components in place and mated. Then go back in and change all the distance mates in one go in the equation manager. Maybe this won't work though and Deepak's suggestion will work better.
A quick solution would be a macro with predefined value, just select the two faces and run the macro via keyboard short cut, toolbar button, etc.
You have my attention now. How can I try this? I know <0 about Macro's.
Here you can read about API/macros: SOLIDWORKS API Help
And here are two link that can help you
Add Distance Mates Example (VBA)
Of course you would have to tweak them to suit your needs but once this is set up, it would be more faster than your current workflow.
The Macro's are way beyond my abilities or comfort level. It looks like I am back to typing .016 and being content. Thanks for the information. I will keep trying to learn more about the macro process.
I'll see if I can make one for you over weekend.
Thank you Deepak! I look forward to learning something new.
OK here is your macro. To run this extract the attached file to a know location. Now open up an assembly file and select faces from two different components. Now go to tool > Macro > run and browse to the extracted SWP file. A distance mate with .016" value would be added between the two components selected faces.
If this works as expected then you can create a keyboard shortcut, mouse gesture or toolbar for the macro to run more quicker and efficiently. Here is how to do that Assigning a Macro to a Keyboard Shortcut or Mouse Gesture
I am having trouble extracting the files. My 3Dconnexion software is trying to extract the zipped files. I will keep trying! Thank you for the help. 
Go ahead and extract the SWP file to desktop and then open via macro button on the SW.
This is one thing this system lacks. When i started on this system 2 years ago I was surprised they didn't have this option. System I used be on it could save the 3 relations with the part. So next time you drag it in, it prompt you to relate it. And it stored it offsets.
Todd Bush wrote:
This is one thing this system lacks. When i started on this system 2 years ago I was surprised they didn't have this option. System I used be on it could save the 3 relations with the part. So next time you drag it in, it prompt you to relate it. And it stored it offsets.
There is something similar here: 2017 SOLIDWORKS Help - Mate References
And maybe you are on to something.
Worth Berry , I wonder if you could do the following:
Create a part.
Add mate references to it
Save it as a template.
Then you can use that template to create your next part, and hopefully the mate references stay linked. Then, when you drop your part into your assembly it will mate it automatically with the correct offset.
I will try it and let you know. Stay tuned....
OK, I am not sure that this will work the way you want it to. Reference mates are tied to the geometry.....and since the geometry will be changing, you would have to redefine the reference mate every bloody time. OK...scratch that!
This isn't what I described.
Yeah, it turns out that Mate References are more limited that I expected. When I first posted this, I thought you could use a distance mate with it to do something similar to what you described........but you can't.
Hello,
If the 1/16th offset is off a common face, then you can create a reference plane in the part that's offset from the face.
Then select this plane instead of the face and select the required face of the other part.
You can hide this plane in the part and select it within the assembly tree.
If you wish, you can rename this plane to a common, yet descriptive of its usage, name so it's consistent across all parts.
Now the mate is a coincident.
Cheers,
Kevin
Edit: Alternatively and especially if you must select different faces on different occasions, you can create an offset surface that has all of the offset planes built into one feature:
Select the part faces that may be used as an offset and start the Offset Surface command (or start the command and pick).
Here's a 3 face surface with red applied for easy spotting:
Kevin, I do this very thing with some of my parts now. I still have to manually input the .016" distance to define the plane on each part. I think changing the spin box increments may be the easiest fix if I can't figure out the macro from Deepak.
This is an example of what some of my CNC frames look like. This is a banquette for seating in a commons area of a large hotel. I know this is simple compared to what most others can create, but I enjoy it.
I had made similar seating frames long back though their design was different.
Just so you know.....I also tried the following, thinking it would be easy.
Creating a dummy part, adding a bounding box to it. Then create 6 planes, each offset from the bounding box 0.016" in the 6 directions. Then saving it as a template.
Then, to create the real part, use the template and then update the dummy part to be your real part.
I thought that this would just move the lines from the bounding box, which would move the planes, but it doesn't. It actually changes the ID of them so that the planes lose their reference and need to be repaired.
I though that this would be a cool way to create planes that would update when your part is changed. But it didn't work as expected.
So scratch that idea.
