I am just making a simple piece of sheetmetal with a pressed nut. I want to locate the centre of the nut at a certain distance from the edges, but it seems that is not possible with the available mates. Can anyone explain how I would locate the nut where I want it in the picture please?
..or use the axis..
Yes something like this is what I was looking for. However I forgot to mention that the parts I would like to mate together are not actually in an assembly. I have inserted a part into another part and have only limited mating options available to me (under the 'Locate part' panel') Is there some way to expand the list of locating/mating options available to me so I can use a distance mate on the axis in this scenario?
yeah,,, I did not read/look well enuf to see it was at the part level... what Dennis Bacon shows is the way to go about this.
..will add/show, as Swapnil has mentioned and pointed out, when inserting a part, you can add features... like the nuts default planes.. then you can locate/constrain via the planes/faces..
Hi jacob,
Please see the image below, you get distance mate optin in "part in part"
To get this window, select part -> select edit feature -> Locate part with Move/Copy feature
You mention using the nut axis to make planes, but forget to mention using the axis for a mate?
Hello Jacob,,, It is really strange that you would want to place a clinch nut (press nut) this way. You do realize that the nut requires a hole to go into. You could weld the nuts on but I have difficulty imagining a reason for doing so although I have done just that on occasion. I suspect that what you really want to do is place your hole (or holes) with the hole wizard or cut extrudes, and use the dimensioning tools to locate them. Then you can insert the nut into the part and place it like you would in an assembly. Works just as well as in an assembly especially if the nuts have mate references. If for some strange reason you don't want a hole you can sketch a point or points, dimension them and use that sketch for a sketch driven pattern. Check out my attached file, I have used both methods. If you work it correctly the descriptions and qtys will show up in you bom also....... Are you using a smart component for a nut? One that will place the hole also?
Jacob, after you placed one set of constraints, hit the "add" button so you can do some more...
Steve C
Thanks for all the advice guys.
Dennis I have put in the clinch nuts without holes as they serve as bolt anchors inside a liquid vat. They will be pressed and then welded in place.
What I have done is simply created some sketches on the surface of the sheetmetal and did a concentric mate with the nuts, like Dennis pointed out. Naturally I could dimension the sketches where I wanted them, I just thought it was odd that I couldn't do exactly the same process with one of the circular edges on the nut and skip the whole sketching process. That seemed like an obvious option to have which is why I thought I'd ask about it.
Jacob, you're not doing it right. You don't need to sketch anything to do what you're after doing.
Steve C
I like the idea of using a layout sketch. Much easier to control, and dimensions and constraints for the nuts are easily accessible. Also more options available for controlling locactions of full set of nuts W.r.t. Assembly and each other.
Hi Steve,
Without adding planes, I don't see how I would locate the nut where I want with the mate constraints in the 'locate part' feature. I can't distance mate the nut edges from the edges of the sheetmetal as, well it's a hexagon and that just doesn't work. I can't mate the axis to anything. The only way I have been able to locate it was to first make circular sketches, like Dennis pointed out, and then do a concentric mate.
OK, you'll have to at least sketch the circle that would make the concentric hole for the press in nut. I'd go ahead and make it a real hole in the part so the sheet metal supplier would have the correct hole size in the model.
Steve C
Hello Jacob,
If you can use planes and then use a normal distance mate.
If you have revolved around vertical/horizontal line passing through origin, you can use top/front/right planes to mate else you can also add planes to nut passing through the axis of nut.