PDM How to get PDM to track references to Forming Tools?

[bnemec]

Is there an option or setting in PDM to make it track reference from part file to forming tool file?

I still get battered regularly about SW lack of a simple dimple function. But now we have all of these forming tool files in the vault and a bunch of part files that use them in the vault but the vault doesn't show that the part file references the tool file or visa-versa. The SW PDM Add-in doesn't show the forming tool when the part file is open and the Vault view does not show forming tool in contains tab. Further undermining the whole "reusable tool file" concept is the where used tab of the tool file does not show the part that uses it.

I get the feeling that I am alone in the argument that there needs to be a dimple feature in addition to the forming tool method. I griped about it in another thread and it seems I work at the only place that finds the forming tool method a waste of time for ~95% of the parts.
https://www.cadforum.net/viewtopic.php? ... +pdm#p6665

So with everyone using them I assume there's a way to get PDM to track the refs.

[jcapriotti]

Is there an option or setting in PDM to make it track reference from part file to forming tool file?

I still get battered regularly about SW lack of a simple dimple function. But now we have all of these forming tool files in the vault and a bunch of part files that use them in the vault but the vault doesn't show that the part file references the tool file or visa-versa. The SW PDM Add-in doesn't show the forming tool when the part file is open and the Vault view does not show forming tool in contains tab. Further undermining the whole "reusable tool file" concept is the where used tab of the tool file does not show the part that uses it.

I get the feeling that I am alone in the argument that there needs to be a dimple feature in addition to the forming tool method. I griped about it in another thread and it seems I work at the only place that finds the forming tool method a waste of time for ~95% of the parts.
https://www.cadforum.net/viewtopic.php? ... +pdm#p6665

So with everyone using them I assume there's a way to get PDM to track the refs.

SolidWorks itself doesn't even show a reference to linked library features/forming tools. It only shows the > in the tree as an indicator.

In PDM you could manually link it using "Paste as Reference" so you can at least get a Where-used.

Does SE do some sort of Where-used tracking?

I get it though, in SE, it's dirt easy to create some of these on the fly. I guess from our perspective, the Library feature work well since it represents actual tools we have. If we had SE functionality, engineer's would be sending stuff we couldn't make without buying tooling . I mean, we only have 3 size louvers created over 25 years.

Most of these would be custom in SE I think. I have really looked into how it does custom forming tools.

[bnemec]

SolidWorks itself doesn't even show a reference to linked library features/forming tools. It only shows the > in the tree as an indicator.

In PDM you could manually link it using "Paste as Reference" so you can at least get a Where-used.
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Does SE do some sort of Where-used tracking?

I get it though, in SE, it's dirt easy to create some of these on the fly. I guess from our perspective, the Library feature work well since it represents actual tools we have. If we had SE functionality, engineer's would be sending stuff we couldn't make without buying tooling . I mean, we only have 3 size louvers created over 25 years.

Most of these would be custom in SE I think. I have really looked into how it does custom forming tools.

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I can defiantly understand that some places wouldn't want random dimples and gussets made. Like you stated you have press tooling that does the features that are available. So engineers can only do features that forming tools exist for. In our case we don't do that. We have only a few break press dimple tools, vast majority of the parts that have dimples or gussets are die ran so the tool that makes the shape is in the progressive die that makes that part (or maybe a couple from that one tool) If there happens to be other parts with same dimple but run from a different tool we DO NOT want them to share the forming tool file. Simply because if one tool is modified and the forming tool file is actually updated it would potentially (if the files would reference the tool and update) update the parts that are ran off other dies that weren't sent out for the same change.
On the flip side, for prototyping new shapes on laser and break our tool room can whip up some pretty darn good "soft" tooling for the breaks if we need to go that route. So custom dimples when needed really are no big deal here. Well, they didn't used to be, but they are now thanks to SW not supporting them. Insert dull stick in eye emoji.

Solid Edge has similar function to the forming tool thing in SW, we just never used it.

SE has some Where Used through Design Manager application. It's a great tool if you're not using some PDM. If you have solidworks PDM do not use Design Manger to make changes because it will make a hash of the files in the vault. This where used functionality was not indexed before ST9. I called it "brute force" where used, and it would open every file in the folders you selected by the file types you selected looking for refs to the target file. In ST9 they started what they called Built in Data Management BiDM. It was a big deal for some, but it was useless to us because our file shares were on a NetApp appliance, not Windows Server. SE BiDM relies on Windows Indexing Service which must be configured on the file server. NetApp doesn't support Windows Indexing Service so we were still in the dark ages. One cool thing however is for this to work SE had to expose their file refs and properties to Windows so they could be indexed. So now you can add a column to File Explorer called SE OLE Links to see the references. That is like the Contains tab in PDM if you like. Once that is all indexed you have a fast where used.

So after all of that jabber I still don't have a good way to track ref to these darned forming tool files we keep creating that are used in one file? Manually adding a PDM reference is not reliable data as it relies on the users to do this. We're limited out on change saturation as it is. I just don't have the energy to get all of them to do this consistently while they are still getting over the hump of a new CAD system and PDM. Maybe I'm wrong

[jcapriotti]

I feel your pain. And I admit, the Dimple, Louver, tools in SE are awesome, really easy to use. We evaluated SE vs SW vs MDT way back in '97. MDT was out early and SE vs SW was a tossup for which we selected SW base on a vote. SE had better sheet metal even then and SW tried over the years to catch up. They made strides in making it easier versus the old "Insert bends" method but they are still a little behind.

[bnemec]

I feel your pain. And I admit, the Dimple, Louver, tools in SE are awesome, really easy to use. We evaluated SE vs SW vs MDT way back in '97. MDT was out early and SE vs SW was a tossup for which we selected SW base on a vote. SE had better sheet metal even then and SW tried over the years to catch up. They made strides in making it easier versus the old "Insert bends" method but they are still a little behind.

Feels like SW is about 10 years behind SE in the sheet metal department. This is a simple part, shouldn't be that difficult to make a nice maintainable model. I thought I was on a role with a decent plan to model this part then I get this:

I'm about to throw care to the wind and just start tabbing and hacking. I like a feature tree that tells a story. Not one that leaves the next person thinking WTH?!?!?!?

[jcapriotti]

I'm guessing at dimensions so I may be missing something. You did two Swept flanges which is meant for more of a stamped like operation. In this case I used a Miter Flange (although multi selecting edge flanges should work and have almost made the miter flange obsolete).

I did the cut on the end but didn't get the weird bend issue, although I have seen that in the past. Can you post your part?

[bnemec]

I'm guessing at dimensions so I may be missing something. You did two Swept flanges which is meant for more of a stamped like operation. In this case I used a Miter Flange (although multi selecting edge flanges should work and have almost made the miter flange obsolete).

I did the cut on the end but didn't get the weird bend issue, although I have seen that in the past. Can you post your part?

It appears the training I took over 2 years ago has faded. I should not be using the Swept Flange, that's not even sheet metal feature. What you said made it clear, it's more stamping op, kind of.

image.png (17.3 KiB) Viewed 3702 times

[bnemec]

I'm guessing at dimensions so I may be missing something. You did two Swept flanges which is meant for more of a stamped like operation. In this case I used a Miter Flange (although multi selecting edge flanges should work and have almost made the miter flange obsolete).

I did the cut on the end but didn't get the weird bend issue, although I have seen that in the past. Can you post your part?

I remember this from earlier attempt but I don't recall exactly how I got to this point, just that I couldn't do the cut. Your gif shows "End Cut" feature. I cannot find that and the command search has no results. Or did you just rename the feature instance?

I tried all the different option combinations and cannot get this to cut.

[jcapriotti]

I remember this from earlier attempt but I don't recall exactly how I got to this point, just that I couldn't do the cut. Your gif shows "End Cut" feature. I cannot find that and the command search has no results. Or did you just rename the feature instance?

I tried all the different option combinations and cannot get this to cut.

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It's just a Cut Extrude....I renamed it so you could tell what it was.

Can you upload the file?

[bnemec]

It's just a Cut Extrude....I renamed it so you could tell what it was.

Can you upload the file?

I cannot upload the real one, blanket policy on CAD data. I'll need to make an example to upload. Had to close SW and restart. Then noticed I had a couple things tied to the imported geometry so cleaning those up first just in case that's causing issue.

[bnemec]

Looks like I selected the wrong face for the sketch that defines the Extruded Cut to be on. I had put it on the face that doesn't move during the unfold/fold. If I redefine the sketch plane to be one of the flats of the Miter Flange then its ok. I suppose it's still learned habits from SE into seemingly arbitrary things. In SE when I have the option, I use geometry that's not moving, it just felt safer. I need to think different to use SW.

Thank you for the time you put into helping.

[jcapriotti]

Actually I selected the same face you did using the same rational, the largest fixed face. Still no bend issue but either it's some minute geometry difference from my roughed together sample or the version I'm using (2022).

[bnemec]

Actually I selected the same face you did using the same rational, the largest fixed face. Still no bend issue but either it's some minute geometry difference from my roughed together sample or the version I'm using (2022).

That's not good Jason. I was fine with being wrong and changing to the rational that I had to put the sketch on the face that was getting the cut.

Hearing that my rational of large fixed face is acceptable but the SW behavior is pseudo-random is worse than being wrong.

Maybe they fixed it between 19 and 22; I have something to look forward to.

[jcapriotti]

That's not good Jason. I was fine with being wrong and changing to the rational that I had to put the sketch on the face that was getting the cut.

Hearing that my rational of large fixed face is acceptable but the SW behavior is pseudo-random is worse than being wrong.

Maybe they fixed it between 19 and 22; I have something to look forward to.

That's why I was hoping I get the file to see if 2022 fixed it. I also have access to 2019 and 2020. Maybe you can cut away all but the end?

Anyway, I have seen the weird bend thing once or twice so maybe its an older version issue.

[bnemec]

That's why I was hoping I get the file to see if 2022 fixed it. I also have access to 2019 and 2020. Maybe you can cut away all but the end?

Anyway, I have seen the weird bend thing once or twice so maybe its an older version issue.

Understood. I made a dummy file that fails the cut just like shown in the gif. I saved it with the sketch on the large fixed face and the cut failed. We're on 2019 SP4. I have not yet installed newer versions of SW, it's on the list but not at the top.
Anyway, I attached the file.

I've been making new file over and over trying to test various things. Applying our gauge table, custom bend radius (I didn't make the part, I just have to remodel the existing), and the height of the edge that becomes bend material. I think I've ruled all of those out. File 0004041.sldprt is about as simple as I can get it. square tab, miter flange (with outside dimensions being the design intent), unbend, sketch and failed cut.

[SPerman]

I am on 2020 SP5. For part 4040, I picked this face for the extrude cut sketch plane and it worked.

If it is a version problem, it wasn't fixed in 2020. It will be interesting to see what Jason finds.

Edit: I can pick any other face and it works, but not the stationary face.

[berg_lauritz]

Understood. I made a dummy file that fails the cut just like shown in the gif. I saved it with the sketch on the large fixed face and the cut failed. We're on 2019 SP4. I have not yet installed newer versions of SW, it's on the list but not at the top.
Anyway, I attached the file.

I've been making new file over and over trying to test various things. Applying our gauge table, custom bend radius (I didn't make the part, I just have to remodel the existing), and the height of the edge that becomes bend material. I think I've ruled all of those out. File 0004041.sldprt is about as simple as I can get it. square tab, miter flange (with outside dimensions being the design intent), unbend, sketch and failed cut.

image.png

What do you want to cut exactly?

As a general rule you should do a normal cut in this case & use a contour.

[bnemec]

What do you want to cut exactly?

As a general rule you should do a normal cut in this case & use a contour.

Interesting; I have yet to be able to use normal cut on this part, I cannot select a face. Just get the error "Please select a sheet metal side face that is not already normal to the sheet metal body." If this needs to be done with Normal Cut I'll go learn how that feature is supposed to be used.

As for the cut, I have to replicate the geometry from the preexisting Solid Edge model "exactly". It's very very close to what is in the gif and screen shots.

[berg_lauritz]

Interesting; I have yet to be able to use normal cut on this part, I cannot select a face. Just get the error "Please select a sheet metal side face that is not already normal to the sheet metal body." If this needs to be done with Normal Cut I'll go learn how that feature is supposed to be used.

image.png

As for the cut, I have to replicate the geometry from the preexisting Solid Edge model "exactly". It's very very close to what is in the gif and screen shots.

This i.e. works for me. I'm on 2021 SP4.

[bnemec]

Screenshot 2021-11-16 102722.png

This i.e. works for me. I'm on 2021 SP4.

Ah, you meant check the "Normal Cut" option, not the Normal Cut Feature. I've been trying those 3 combinations (optimize on/off).

I might see the problem, I didn't select through all, I left it to thickness.

Edit: Looking back I can see that changing the extent type should have been one of the first things I tried when the feature failed. IIRC "Set to thickness" was usually the safest in SE. I try to not have "Through All" as default because sometimes it cuts something added later in time but earlier in the tree, and because I've heard several times that each "Through All" takes a bit more computation to look for all the geometry it might intersect on each rebuild.

[jcapriotti]

For the 4040 file the cut works fine but I couldn't fold it back up. This little edge is causing it. If I notch it out it works fine.

[bnemec]

For the 4040 file the cut works fine but I could fold it back up. This little edge is causing it. If I notch it out it works fine.

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That stupid little vertical edge... it's a long story that's probably not worth the time to read. Short(er) version is I try to model so that a simple change in thickness or custom bend radius doesn't cause an undesirable, subtle change in the fit/form/function of the part. In this case it appears the custom radius, applied sometime after first creation of the part, caused the flange width to not be nominal but it went unnoticed. Sometimes it's a compromise.

[jcapriotti]

Yeah, we had fun 20 years ago fighting with both SolidWorks and manufacturing over sheet metal flat patterns. Prior to SolidWorks, we used Catia but not it's sheet metal module, just regular features. Flat's were manually calculated and drawn in 2D and all dimensions rounded to the nearest 1/16 of an inch. Manufacturing would push back when we modeled the part in SW and an ECO would have us redo the drawing and the flat dimensions were now no longer rounded. They wanted us to fake the flats to match the old rounded numbers and we refused because it meant we had to tweak bend allowance on each bend to get it to come out. Eventually we won that battle but not without drawing blood.

[berg_lauritz]

For the 4040 file the cut works fine but I couldn't fold it back up. This little edge is causing it. If I notch it out it works fine.

image.png

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forgot to mention that. Always causes issues & I automatically made a tiny cut there....