Sharing parts between subassemblies/jobs in real life

[dogarila]

Suppose we have to design an assembly line with 5 stations. We will call the job A1000 and the stations will be 100, 200, ..., 500. The main layout of station 1 will be
A1000-100-000. Then we call subassemblies in a station using the middle digit of the station number like
A1000-110-000
A1000-120-000
and so on for station 1
A1000-210-000
A1000-220-000
and so on for station 2
and so on to station 5

Details of these subassemblies are A1000-110-001, -002 ...

Suppose we have 2 subassemblies quite similar on two different stations, with many identical details. For example A1000-220-000 and A1000-420-000 share 9 identical parts, A1000-220-001 to A1000-220-009 are identical to A1000-420-001 to A1000-220-009.

Now, I design station 2 which includes A1000-220-000 with its 15 parts (9 similar with A1000-420-000). When I get to station 4 for subassembly 420 I copy 220 using SW Explorer then modify de parts that are no common with 220.

When I create the drawings I will create one for each part called A1000-220-001.sldrw....

When I get to create the drawing for 420 I would like to use the drawings already created for 220 and not redo them from the scratch.

We inherited this system from AutoCAD where it was faily easy to generate similar drawings by changing the information in the title block.

Looks like SW requires a different way of thinking. I would like to be able creat one part with one drawing used in several subassemblies through out a job, or even shared within more than one job, eliminating any duplicate work. How should I number them? Lets say part P1AAA (sensor bracket) is used 2 times in A1000-220-000, 4 -times in A1000-340-000 and 2 times in A1000-420-000. These subassemblies are released at different dates. How do I make sure that in the end I will get 6 parts from manufacturing and not 2 or 4?

Regards,
Andrew

 

[DigiBob]

I would create that part as a generic part with it's own unique drawing number. In the title block I would use the "next higher assembly" area to list all the subassemlies and quantities per assembly. On the NHA subassembly drawings you would put this part number in the parts list. Whenever you use this part again on a new subassembly, you would need to update the next higher assembly block on the generic part drawing.

Bob

 

[BBJT]

This may help you out.

This is what we do when have a part, 220, that is complete with detail.

Scenario #1.....220 complete with detail and 420.sldprt is not yet created.

When is comes time to create 420 we open the 220.slddrw and do a file Save-As. We rename the drw to 420, the select References in the Save-As dialog and double click on the part name, under the new path name area, and rename it to 420. You can browse and put the new part in your 420 folder along with the drw. What SolidWorks does is create an identical copy of the part and drawing with its new name in the directory you specified with the links intact.

Scenario #2.....220 complete with detail and 420.sldprt is already. If 420 was created by doing a Save-AS on 220 you are in luck. Open up the 220.slddrw, do a Save-As 420.slddrw. DO NOT do the references step that was mentioned in the first scenario. If you do it will over right your existing 420 model with your 220 model.
You are now looking at 420.slddrw which is still looking at the 220.sldprt. Right-click in any view op the drawing and open the 220.sldprt. In the model go under the File pull down and select Reload. In the reload dialog pick replace and select the 420.sldprt and OK. Go back to the drawing and you will see it know pointing at 420.

The key to these scenarios are using the save-as. It sounds like you already know that parts are going to be similar between assemblies. Create one part(220) and do a Save-As to create the similar part(420). If you do not do the Save-As there are two big down falls that come to mind.
1.) Your duplicating your efforts by creating the same model twice.
2.) By doing a Save-As the model will have the same internal ID. If your create 220. Then start up a brand new part and create the exact same model form scratch the internal ID will be different. In this case if you follow Scenario #2 the dimensions will be dangling in the new drawing. SolidWorks does notify you, in this case, when you are doing the reload and replace that the internal IDs do not match. Same goes with assemblies, if you try and replace a part with another part with a different internal ID, even know they are identical, the mates to this part will break.

As you can see a whole book could be written on this subject alone. I hope this helps.



BBJT CSWP