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

Reply to
bill allemann
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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

Reply to
Wayne Tiffany

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

Bill

Reply to
bill allemann

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

Reply to
Tin Man

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

Reply to
bill allemann

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

WT

Reply to
Wayne Tiffany

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

Reply to
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

Reply to
bill allemann

located at a given coordinate, or a distance from an edge, whatever?

stick with traditional assemblies instead of weldments.

Reply to
Tin Man

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

Reply to
John H

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