[sideburns5]

Greetings,

I have begun the CAD stage of a machine design that I have been working on for the past few months, and am in the process of putting together the assembly of the components I have drafted so far. I am not a new Solidworks user, but I am not a pro either. The problem I'm running into is when I go to mate the v-groove bearings to the linear rail, the part shows the (-) symbol in the assembly tree to denote partially constrained, however I am not able to move the part.

I am mating the 1 conical bearing surface of the bearing to the corresponding face of the 90, and the other conical surface to the opposite face of the 90. Both mates are forced to Tangent which I logically would have thought was correct. If the conical surfaces are being forced to remain tangent to the each side of the 90 degree surface, the bearing should be able to slide along the length.

Something isn't right though, because if you grab the bearing component and try to move it in the assembly space, the part doesn't even spin on its access. I created the bearing using a 3D revolve, and have tried making the linear surface with both a typical solid extrusion and a sheet metal bend and got the same result.

I am using Solidworks 2013 if that helps,

Anyone have any thoughts on why this wont work? Or if there is another way to mate my parts? I would rather not have to create planes and mate that way, because it should work without doing it that way (unless my logic is incorrect or I am over looking something).

Any info anyone can give would be great,
Thanks!

[BuckNaked31]

I've never gotten conical shapes to mate well tangentally, I use sketches and planes for mating these. I make a center plane in the bearing file (if you don't already have one) to align the bearing to the angle iron and use a sketch in the bearing part file to bring the v bearing to the face of the angle iron, then hide the plane and the sketcht in the assembly after the parts are mated. It helps when you are drawing a part to visualize how it's gonna be mated in an assembly also...

[sideburns5]

Yeah I typically do try to visualize the part with regards to assembly, and in this case I just don't understand why it would be a problem to do it the way I explained. If I understand what you described, your saying drive a defined plane through the center of the bearing, mate that plane to be parallel with the cutting surface, and then use the revolved sketch to be colinear with the faces of the angle iron?

I can see why that would work, but I'm a little frustrated that it requires a work around when I can't think of any reason why my method wouldn't work. Is it just a software issue? I'm thinking the other way I may have to do it is to assemble the gantry first, and then use only 1 tangential mate per v-bearing for both the top and bottom rail to drive the gantry into its proper location (if that makes sense). But again... it kind of pisses me off that I have to use a work around, at this point I'm also interested in why it doesn't work like it should. If I'm doing something wrong I want to be able to fix it!

[BuckNaked31]

I hear you. Yes, your describing almost my method... There are several ways of doing it. When I first started it took my awhile to draw the parts in such a way that I could skip the plane creation later by using the front, right and top planes to my advantage. One thing for example in extruded parts is to always extrude the profile mid plane, so I automatically have a center plane for mating and mirroring features in the assembly stage later. You can also do that in revolved parts. I make the top plane the center of the part. Then you can mate to the axis of another part without having to create another plane. Also remember that you can mate points to surfaces in the assembly. This way I don't have to create a second sketch, I just use the points in the revolve sketch. I also try to mate planes first before points, the parts are a little more stable that way. I wish you could just select the surfaces like you said. It seems like it should work the way it does in nature, although the planes and sketches method works it seems like a kludgy way of doing it. If you can get it to work, let me know... It was quite a head scratcher for me too, but it did force me to draw my parts differently which helped me out in the long run.

[cygnus x-1]

Most likely the issue is that when you go to click and drag the part, SW can't figure out whether you want linear movement (XYZ position change) or rotation about some axis/point. So it just does nothing. I've noticed this seems to happen with round parts that are partially constrained and both forms of movement are valid. If you want the bearing to slide along the rail you need to constrain the rotation somehow. I know this is the opposite of what you would want in real life, but software in general doesn't deal well with ambiguity.

Is some cases you can also try to click/drag on a different part of the assembly to get the movement desired. So for example if the bearing was mated to a shaft and then the shaft was mated to a gantry, you might get what you want by dragging the gantry itself (instead of just the bearing), because the gantry would likely be constrained such that it can't rotate, and the only option is linear movement.


C|

[sideburns5]

I was wondering if that would be the case, and I just haven't gotten far enough into the assembly to test it yet. I'll try mating a plane on the bearing to be parallel with a x,y, or z face on the table when I get home and see if that has an effect.

I'll report back when I have news!