Weldment ... Insert Part feature

I'm having considerable trouble with the Insert -> Part feature. Location
of the part relative to the rest of the weldment seems almost entirely
incomprehensible. Is there any information anywhere that explains what
features/geometry are usable for doing constraints? The help file reads as
though constraints can be done in a similar manner as in assemblies, but
that is apparently not the case. I've managed to get a rectangular object
located, but I can't get anywhere with a cylindrical object. It seems that
the original planes of the weldment or the inserted part are mostly not
usable?
thanks,
bill

 

When you build a part in the context of the assy, that part's system planes
will be aligned with the assy planes. The advantage of that is that you can
just place those parts into another assy and have them locate properly.
Think of an example of a car. The vehicle 0 body lines are generally
through either the crankshaft or the front driveshafts. Anything built for
the car is referenced to those 0 lines and you can take a part from one
model and stick it into another model and know that the relationship of the
part is correct in the assy.

Now that being said, if you don't care about that in the new part, then
after you create it, just open the part and move the sketches, etc.

WT

 

I know how to do all that in an assembly, but are you saying that can be
done in a weldment?

Bill

 

For any Multi-body part, to move one of the bodies or an Inserted a
Part go to:
-Insert-Feature-Move/Copy
-This dialog has 2 forms:
1) "Constraints" that uses part geometry to locate the body or part.
-or-
2) "Move/Copy Body" that uses inserted values to move the body or
part
-If you're in the Feature Manager dialog box, and you seen a
Constraints button at the very bottom then click it. No you'll be
looking at the "Constraints" version of the dialog.

Note: This is not a "parametric" relation. So if you later move the
base body/part, you'll have to also move the body/part that previously
was moved relative to the base body/part.

Ken

 

What you've described is what I've been trying to use, and it works OK on a
part with flat faces.
If the inserted part is cylindrical, it appears that the only constraint
possible is tangent to a flat face or concentric to a cylindrical face of
the weldment.
An example would be that the end face of a cylinder of the inserted part is
made coincident to a face of a flat plate.
How then can the axis of the cylinder (or the center of the cylinder end)
be located at a given coordinate, or a distance from an edge, whatever?

Thanks, Bill

 

Ahhh, sorry - didn't read the title carefully. :-( Don't know on a wlmt.

WT

 

Solidworks hasn't quite got the manipulation of multi-body parts sorted yet,
though it improved greatly at 2006 (vs. 2004 anyway).

The workaround is to create a sketch on the "fixed body" and add points to
define the centres of any circular parts.
You will now be able to use a concentric constraint between the cylindrical
"moveable" body and any of these sketch points.

PITA but it works.

Regards,
John H

 

I come up with that very technique late last night. I was reading up on
sw2007 and it doesn't look like much
is going on there with weldments, unfortunately. I can see that with
certain odd parts to be inserted, it might be
simpler to stick with traditional assemblies instead of weldments.
Thanks, Bill

 

<<<

If the "Constraints" interface won't do this for you, use the
"Move/Copy Body" interface. With that, as long as you know the distance
the inserted part needs to move from it's present location, just use
the "Move/Copy Body" interface and enter in the value. Personally, I
still prefer this interface over the "Constraints" interface most of
the time.

<<<

If this truely is a weldment, then I'd still say stick with the
Weldment part process, but do not try to make "assemblies" using a
single part multi-body file. That's just asking for trouble now and
later on (i.e. BoM, Ballooning, Detailing, etc...)

Ken

 

We do fabrications as a mixture of assemblies and weldments here.

There are obviously pros and cons of each method, but since moving from 2004
to 2006 I think the pendulum is swinging in favour of weldments. This is
mostly because of the new ability to mate bodies, but as you've found out,
it's not yet perfect.

Doing it with assemblies is a bullet-proof method, but the hassle of having
to make copies of all the parts when starting a new job (based on an old
one) is not at all time-efficient. This would be better (I think/hope) with
data management, which we don't have. Having to do "save as" on each part,
opening it up and changing all the custom properties is a real PITA with
basic SWX OS functionality.

I certainly don't like the suggestion of using "move bodies" - the command
is very limited in itself, and it does not capture design intent.

Regards,
John H