CAD Forum

So I came across this several times now & I never know what the best way would be:

• you have a jig basically for an assembly feature (i.e. bolt holes or cutouts)
• this changes over time, so the jig changes
• how do you define the jig?
  through the assembly feature? doesn't that cause a crazy amount of rebuilds? what if you re-use the jig on a different assembly?
  through the jig feature? but that means, that the jig needs to be in the assembly all the time to show the feature
  make jig & assembly feature independent from each other and risk mistakes esp. across multiple assemblies?

We do a mix of everything currently and it drives me nuts. I want to define a standard for that.

Best practice would be to drive both the assembly and the jig with a layout sketch or SSP (Skeleton Sketch Part). This keeps references from getting tangled and reduces rebuilt time because there is one parent that "keeps the kids in line" instead of allowing tangled sibling rivalries.

As far as reusing the jig in another assembly, that is fine but make SURE it is not defined in any way by the second assembly. To quote @matt: "If single contexts are a thing to be feared by some, multiple contexts just open the gates of hell itself." (edit: see quote here)

Assembly/Part + MasterSketch = MasterAssembly
Insert MasterSketch into Jig.
I do put Jig back into MasterAssembly to check. Of course don't edit MasterSketch and reference the Jig.
It is not perfect. I usually use customer import. So an update means lots of double checking.

mike miller wrote: ↑Wed Jun 30, 2021 3:34 pm Best practice would be to drive both the assembly and the jig with a layout sketch or SSP (Skeleton Sketch Part). This keeps references from getting tangled and reduces rebuilt time because there is one parent that "keeps the kids in line" instead of allowing tangled sibling rivalries.

As far as reusing the jig in another assembly, that is fine but make SURE it is not defined in any way by the second assembly. To quote @matt: "If single contexts are a thing to be feared by some, multiple contexts just open the gates of hell itself." (edit: see quote here)

This brings out the Good luck with SSPs for fixtures/jigs when there are other, unknown future products that will share that tool. You just defined the reason the place I work just does not use any form of top down for production models.

berg_lauritz wrote: ↑Wed Jun 30, 2021 3:26 pm So I came across this several times now & I never know what the best way would be:

• you have a jig basically for an assembly feature (i.e. bolt holes or cutouts)
• this changes over time, so the jig changes
• how do you define the jig?
  through the assembly feature? doesn't that cause a crazy amount of rebuilds? what if you re-use the jig on a different assembly?
  through the jig feature? but that means, that the jig needs to be in the assembly all the time to show the feature
  make jig & assembly feature independent from each other and risk mistakes esp. across multiple assemblies?

We do a mix of everything currently and it drives me nuts. I want to define a standard for that.

Welcome to our world, but it's not just for jigs. We build all of our weld fixtures inhouse. Tool room designs them, they've tried to follow top down modeling methods but it bit them too many times.
The most reliable and transparent to all is for the top level assembly of the fixture/jig to include the top level model of the part it's making. If there are various parts that the tool makes then they all go in there. If you continue to revise parts, and add new parts that use the existing jigs, any attempt of using a master anything will probably crash at some point. That's just what I've seen.

We rarely ever use existing jigs as start-up for new ones, so when I do create a jig, I'll build it as required(using external references if necessary), and then I will remove it and dimension as necessary, in case I need to modify it eventually. This way, the jig doesn't keep an external reference and I don't end up loading unnecessary things.

All depends on what the need is.

bnemec wrote: ↑Wed Jun 30, 2021 4:15 pm This brings out the Good luck with SSPs for fixtures/jigs when there are other, unknown future products that will share that tool. You just defined the reason the place I work just does not use any form of top down for production models.

I'm curious about this. Are you trying to make a single assembly be driven by multiple assemblies? That's the only way I see what your saying working and I'm pretty sure that's a road to a whole lot of trouble.

If you have a fixture that is designed for assembly "A" and the fixture is driven by assembly "A" you can't also have it driven by Assembly "B".

I think if I were doing this I would look for a method, outside of SW, to verify if any new assemblies will work on the fixture. Tie the fixture to assembly "A". Pull all the pertinent dimensions into Excel. Place limits, conditional formatting or something on those dims. Design Assembly "B". Pull the same pertinent dimensions into the same spreadsheet with conditions. Either it fits or it doesn't.

You might be able to go back and alter the fixture, which is essentially changing your limits but you can't alter the fixture in such away that it no longer fits Assembly "A" and thus the fixture will always be driven by assembly "A". Not sure there is a way around that.

MJuric wrote: ↑Wed Jun 30, 2021 5:02 pm I'm curious about this. Are you trying to make a single assembly be driven by multiple assemblies? That's the only way I see what your saying working and I'm pretty sure that's a road to a whole lot of trouble.

If you have a fixture that is designed for assembly "A" and the fixture is driven by assembly "A" you can't also have it driven by Assembly "B".

I think if I were doing this I would look for a method, outside of SW, to verify if any new assemblies will work on the fixture. Tie the fixture to assembly "A". Pull all the pertinent dimensions into Excel. Place limits, conditional formatting or something on those dims. Design Assembly "B". Pull the same pertinent dimensions into the same spreadsheet with conditions. Either it fits or it doesn't.

You might be able to go back and alter the fixture, which is essentially changing your limits but you can't alter the fixture in such away that it no longer fits Assembly "A" and thus the fixture will always be driven by assembly "A". Not sure there is a way around that.

Nothing is driving anything; well, parts and sub assemblies that are in the assembly drive the assembly, so purely bottom up. That is the only way we have found to deal with constantly revising and constantly evolving where used.

If I understand @berg_lauritz description in original post that the part/assembly that physically needs the jig for manufacture will change or be revised over time. Also the jig may be used to make other similar parts/assemblies.

That's the world I've learned to use solid modeling in. In our case it's likely that in a few years the part that caused the jig to be created is obsoleted but the jig is now used on five other parts. The parts may be revised independently or as a group depending on the change requested. The fixture may need to be revised to accommodate new part or changes to the parts, or may need to be revised just for it's own sake (usability maybe) but none of the parts would be revised. Sometimes we revise parts to accommodate needed changes to the fixture (add a hole for positioning pin for example). There is no consistent direction of drive, so nothing drives anything, we model bottom up.

bnemec wrote: ↑Wed Jun 30, 2021 5:41 pm Nothing is driving anything; well, parts and sub assemblies that are in the assembly drive the assembly, so purely bottom up. That is the only way we have found to deal with constantly revising and constantly evolving where used.

If I understand @berg_lauritz description in original post that the part/assembly that physically needs the jig for manufacture will change or be revised over time. Also the jig may be used to make other similar parts/assemblies.

That's the world I've learned to use solid modeling in. In our case it's likely that in a few years the part that caused the jig to be created is obsoleted but the jig is now used on five other parts. The parts may be revised independently or as a group depending on the change requested. The fixture may need to be revised to accommodate new part or changes to the parts, or may need to be revised just for it's own sake (usability maybe) but none of the parts would be revised. Sometimes we revise parts to accommodate needed changes to the fixture (add a hole for positioning pin for example). There is no consistent direction of drive, so nothing drives anything, we model bottom up.

The only way I see that working is in a big table with conditional formatting of some sort. Instead of tying the fixture to an assembly you could tie it the table. Change a dimension in any assembly or model and the table is updated and shows things that aren't going to work.

MJuric wrote: ↑Wed Jun 30, 2021 5:50 pm The only way I see that working is in a big table with conditional formatting of some sort. Instead of tying the fixture to an assembly you could tie it the table. Change a dimension in any assembly or model and the table is updated and shows things that aren't going to work.

I think I understand what you're saying, that could work, but then the users involved need to agree on how to set up the table and understand how to use it. Granted it's just excel, but of the people that design fixtures in the tool room maybe 1/2 of them are fluent in excel, the other half will try to attach it in an email. We just use the graphical tool (CAD) to see the parts instead of a table linked all over the place.

The weld fixture (in our case) is built around what it makes (again in our case this is an assembly, but could be part file) but the fixture model is not driven by the model of what it makes. Then as the fixture is used on more and more part numbers those models are added to the fixture model. This way they can be shown or hidden, colored, whatever. So instead of using another tool (a table) they can just use CAD and have a graphical view. We do a lot of edit in place, but again no driving down the tree. Yes this stinks when we have to move one screw because it requires the edit to be done in all the models affected; there's no move the screw in the assembly and the pc parts all update, we don't do that because then what about all the other places that use those parts? A part cannot serve two masters, it will either work for one and break the other or wreck one and work for the other.

bnemec wrote: ↑Wed Jun 30, 2021 6:18 pm A part cannot serve two masters, it will either work for one and break the other or wreck one and work for the other.

Exactly, so you're really left with finding some other way to "Verify" that everything is compatible and there are probably a bunch of ways to do that.

MJuric wrote: ↑Thu Jul 01, 2021 8:00 am Exactly, so you're really left with finding some other way to "Verify" that everything is compatible and there are probably a bunch of ways to do that.

Yes. Verification is done graphically in the model and drawing views. I agree with the top down or master sketch/model/etc. methods are nice in that they automagically keep all of the models in line and then verification is pretty much done as part of the modeling process. That works nicely when the file references make a nice tree with few links to other assembly structures but managing the in/out context references becomes nearly impossible if the file refs are more of a cobweb than a tree.

Did I hijack this thread or are we still helping @berg_lauritz ?

You are still helping. It gives me something to think about. We do have some items, where the jigs are easily replaceable & they are bound to the assembly & it makes sense this way (mainly textile jigs). There we only have to pay attention to a possible mirrored side & that is it.

But other jigs are exactly as you described (welding jigs for various parts/assemblies, sometimes drilling/manual CNC jigs) & there is no clear path. Top down seems appropriate, but dangerous & we have to weigh the risks & I love to hear your opinions on that.

Do you keep them (the jigs) in each assembly?

Okay, I have a follow up question here:

If we use a SSP - do I insert the SSP into the part too? Because in this case I don't want to insert it into an assembly. Or is this bad practice & I should just make a small assembly, that will be dissolved, where I insert the SSP into?
I only ever did it, when I inserted it into an assembly & linked the parts through the assembly to the part...

I avoid assembly features. I do all feature in part and use config. So Master Sketch is in all the parts.
I'll put MS in assembly to locate/constrain parts if necessary.