Assembly error and mate problems 1

[gunnykiln]

Thanks for all the help I have had on this site so far.

1. On my project I could not mate two parts in assembly. One was essentially a block with screw clearance holes, the other was a plate with tapped holes. I could mate two of the holes with concentric, but when I picked the faces that would be coincident (Bottom of block and top of plate) I was given an error that the two faces were not parallel. The problem was one face was .000378 deg off being horizontal. That is such a ridiculously small number for what I am making is there a way to increase the tolerance of mates? Or at least to tell the software that .000378 deg is close enough?

2. So I am working on another project and for simplification purposes lets say I have two plates and two hinges to connect them. I make my "hinge" as a separate assembly since it is something that we use all the time. On my project assembly I insert my first plate, then I insert my hinge sub assembly and mate with screw holes to "plate 1". Then I insert my 2nd plate and mate to the other end of the hinge sub assembly. Very simple" two parallel plates attached by a hinge.

Now when I try to "work" the assembly (rotate one half of the hinge and plate2 about the hinge point with the move component command) it will not move. So I go check the "hinge" subassembly and I can "work" one half the hinge so there are no restrictions there. I go back to my project and double check my mates and there doesn't seem to be anything holding it up. It seems to be problem of using sub assemblies within another assembly. It just seems like such a stupid a problem I must be missing something in order to make it work. So how can I "work" this assembly?

 

[CorBlimeyLimey]

1) To answer you question ...No. What you should do is go back through you features & geometry & correct the error. Somewhere you probably have a plane or axis or ??? which is not aligned as it should be.

2) Check the Help files for Flexible sub-ssemblies


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[Timelord]

gunnykiln,

Problem 1: The holes must not be square to the surfaces you are trying to mate. Go back to the parts and make sure you put the holes into the faces you are trying to mate. If you didn't put them in square to the surface, by not using the face as the sketch plane for the holes but used some tilted plane, then they won't mate in the assy.

Problem 2: Right click on the door subassy in the your top assy and under properties check "flexible". You must have this set to make motion possible inside an subassy.

Timelord

 

[MElam]

Are the faces supposed to be ".000378 deg off being horizontal"?

If not, at least one of the parts is wrong somewhere and should be fixed as stated above.

If they are not supposed to be truly parallel, you just need to use an edge instead of a face to mate the parts.

 

[gunnykiln]

Thanks for the quick replies.

The .000378 deg wasn't intentional, but its also not significant. But I did go in an correct it in the part model.

On the hinge question: I clicked the properties/flexible option and it gave me several mating errors that I am trying to fix.

Each side of my "hinge" mates (via concentic screw holes and coincident mating surfaces) with a plate. The errors I am getting are are said to over define the assembly.

But if I delete plate2 I can move the hinges and the errors go away.

 

[Theophilus]

Are you creating references within the assembly? In other words, to make sure holes are truly concentric, sketch the holes in your hinge in the assembly and use the centers from the screw holes in the plate (or vice versa). Also, define the hole centers with intentional dimensions (no blue stuff in the sketches).

Right is right. A little off, and you're going to have trouble. SolidWorks uses absolutes regarding fit and form--it must, or it would be totally invalid.

You also might want to check the other thread regarding assemblies that is in this forum now for some good practices in assemblies concerning mates.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[macPT]

SW is a tolerant tool and that also means dangerous.

It will not verify your design, but give you clues of things that can be wrong. And if you find things that are wrong you must fix them properly. Don't leave your work half way done. Otherwise you risk to have a design modified unexpectedly (one common and good example is leaving the components of an assembly not fully constrained).

In this case you want the faces to be parallel but SW knows that it's not possible, given the earlier constraints. For you the error is small enough, but not for SW: the faces can not paralel - period. You can live with that and even find an alternative mate that will let you proceed with your work. But your model still contains an unknown error. What if you change some dimensions in your part (a diameter, a length,...)? The error can cause a result significantly different from expected and even the part or assembly to fail.

Do the work only once. Do not ignore the error. Go back and fix it. You will save time and headachs in the future.

Regards

 

[SBaugh]

This is why I use planes versus faces at almost all costs.

http://www.scottjbaugh.com/Design_Portfolio/In-contexted_Plane_mated_assembly.zip

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

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