Constraint: mate edges 1

[kierancoghlan]

In an assembly file, you can mate two edges. You can also define an offset for this constraint, presumably so that you can make the edges parallel at a distance.

Thing is, you can't define in WHICH direction the offset applies...

Anyone know how to achieve this? I have two parts, and I want to constrain two z-axis edges, with an x-axis offset, but the offset value seems to only apply in the y-direction.

 

[malaycobra]

I am new to Inventor, but I think you just need to use a negative value to have the offset in the opposite direction.
Hope this helps!

 

[cadranger]

kierancoghlan,

You can't do it, not in 5.3 anyway. If you want the two edges to be coincident then the mate contraint will work but the two parts will rotate about each other around that constrained edge. If you want the edges to be offset you can select an edge and then a face (perpendicular to your desired offset) and give it a positive or negative offset. This will only mate the parts in one plane requiring more contraints. The best method is to mate flush two sets of common faces that share the edge and then mate with offset the last two common faces (this last one being the faces that are perpendicular to the desired direction). This method allows the most freedom for editing constraints should you need to offset in any direction.

 

[autocol]

As you work with Inventor you begin to learn which constraints are the best and which could use a little help. You've found one that could use some help...

The problem is constraints with multiple solutions. Mating two edges with an offset has an INFINITE number of solutions (or maybe 360 if you want to round to the nearest degree ;-) )

To mate two edges with an offset you also need at least one more mate or angle constrain to remove possible solutions that are not the one you want.

But here's my suggestion with using constraints with multiple solutions:

NEVER USE THEM!

In the example you've asked about, I would place a sketch in one of the parts (or modify an existing sketch) place a sketch line which you can easily dimension into position, and leave that sketch visible when you finish-edit the part.

Then mate the edge to the visible sketch line and you've got an un-ambiguous, single solution constraint.

I never use tangential constraints either, for the same reason. I never have constraints bite me later as a result of my constraining methods...

Hope that helps...


Col.