Can assembly constraints tolerance be adjusted?

[Barry1Lau]

Inventor 2012 on Win7.

I am trying to assemble two parts by locating with dowel pins.  The parts are constrained by insert constraint on the first dowel holes and mating the axis of the 2nd dowel holes.  The grounded part has the dowel holes located at an angle relative to the X-axis using X and Y coordinates from another feature.  the part being placed has the dowel holes located on the X-axis in the model.  When I measure the distance between the dowel holes in the grounded part with a 4 decimal place value (in inches) then set the distance between the dowels on the placed part to that value.  Apparently this is not a close enough match for the axis mate contraint to succeed.  Is there a way to back off the precision on the constraints so that I can keep working?  I really don't want to deal with 7 decimal place dimensioning.

[JDMather]

An assembly file (*.iam) is only a list of hyperlinks to the part files (*.ipt) and a record of assembly constraints (and a bit more).

You must include the part files.

I do not know of a way to introduce a tolerance to constraints, but this is how I handle this situation -

1. preferred - model using the same dimensioning scheme in both parts.

2. if you can't do that for some reason - apply a tangent between pin and hole in first part and pin and hole in second part.  (actually the tangent can be placed directly between the two holes)

[Barry1Lau · Accepted solution]

I couldn't get the tangent function to work correctly.  The outside tangent function worked okay but the nested tangent does not (could be a bug).  The "solution" that I found was to mate the base part dowel axis to the placed part X-axis face used for locating the dowel hole Y-axis dimension offset by that amount.  Then any residual mis-match of the centers can be adjusted on the placed part.

[coreyparks]

Generally this is an excellent time to use adaptivity.  If you leave the second hole unconstrained in the sketch and then make that feature adaptive you should be able to constrain the part and the hole will move to the exact location required.  If you have never used adaptivity take a look in the help files some assitance.  Take a look at the attached files and you will see part 2 has no dimensions locating the holes but they are aligned exactly with part 1 even though the holes in plate 1 were placed totally randomly.  Go ahead and change the dimensions in plate one and then update the assembly and the holes in plate 2 will move to follow.

[Barry1Lau]

I couldn't get this to work very well.  I wasn't able to open your file maybe because it is in a newer format than 2012.  I tried making the placed part adaptive in the assembly then mating the two hole axis.  The success tone was emitted but then "the failed constraint" dialog box displayed which meant that it didn't take.  My offset mate system seems to work okay.  It is too bad that Inventor doesn't allow an angle constraint of formed planes (created from a pair of axis on each part) like MDT did.  It's also too bad that Inventor give an angular measurement with the distance like MDT used to do and AutoCAD still does.  I will have to fiddle with the adaptive command to see what happens.  If the undimensioned feature will hold its location when the part file is opened so that the required dimension can be determined, that would be helpful.

[JDMather]

After reading this - I recommend that you attach your assembly here.

I suspect there are some tips you need to avoid developing some bad habits in the transistion to Inventor.

[Barry1Lau]

Here is the assembly (hopefully).

[JDMather]

Have you experimented with mutli-body solids?

This looks to me like it would be much easier using multi-body solids AND that would be a technique more familiar to MDT user.

Design the bodies in a single file and then push out the assembly and individual parts.

Multi-body all but eliminates assembly constraint problems (unless you have relative motion between components - and usually this is limited).  I think multi-body is the way to go.

[Barry1Lau]

I do that sometimes when starting with a fresh tool. In this case, I am recreating something that already exists and has real parts. The amazing thing is that the assembly constraint seems to be precision to much more than 4 decimal places. When I measure the distance from the centers of the holes it is less than .0005" which is about as precision as we specify for machining. A pretty picture and sub-nanometer tolerance is nice until you actually have to build something. I just don't understand why the constraint has to be so tight.
Thanks for your time,
Barry Hazel
Mfg. Engineer
Lau / Ruskin Company
Rochester Plant
(574) 224-5200

[t_stramr · Accepted solution]

If you want to bring more flexibility to your constraining you can apply flexible flag to constrained components. This will influence all constraints that consume these components. If you want to be more specific, you can use constraint limits for each individual constraint. Specifying min, max range will accept all constraint solutions within this range. Allowing Resting position will make a constraint to work like a spring. You can find constraint limits in extended varion of constraint dialog by pressing button << at right lower corner of the dialog.

Thanks,

Robert

[Barry1Lau]

Setting min/max limits on the mate constraint is the solution that I came upon around 3AM.  I wish that I had read your response earlier, it would have made sleeping easier.  Thanks for the help.