CAD Forum

bnemec wrote: ↑Thu May 27, 2021 3:13 pm I had to dig back in my notes now to see where we were with toolbox. At @JSculley mentioned, toolbox is not available in Standard which I had forgotten about and was helpful reminder because I wasn't looking back to before we purchased SW. It was a matter of chicken and egg. We couldn't get contextual examples of how we would set up TB and how it would work in our case with PDM and revising hardware and so on. Can't test it without buying it. Since we heard a lot of "hardware aren't revised" type comments we decided it wasn't for us. And, because there was nothing else in Pro or Prem that we needed we bought Standard.

If you go back far enough, Toolbox wasn't even developed by Solidworks. It was developed by Cimlogic, and sold to SolidWorks at some point. It was one of the first (and most popular) 3rd party partners, and one of the first to get purchased by SW.

bnemec wrote: ↑Thu May 27, 2021 2:36 pm That is good news as we went to great lengths to make sure the proper geometry was used to locate the parts, even colored the faces that are to never change no matter the length of thread (full or not) or head style.
What I'm not sure about is we thought is was a good idea to organize the screws by size then length so all the actual part number configs are buried under generic "folder" configs. We were learning as we went and learned a little too late there there is no way to move them around.

That's a minor issue though. When you are changing the config using the drop down, it's a flat list with indenting anyway:

The hope was that each of the dispersed files would only have one config, but keeping the name the same is not a problem. The Replace Component is what scares me. Many files, Many components, many of them in released state (revision control).

I wouldn't do that. I would keep configured models, but limit each file to one general screw type. I went a step further and split between fine and coarse threads. I regret it sometime when I want to swap a #10-32 UNF for a 1/4-20 UNC, but keeping the config count manageable in each file was more important.

As for your released files, there's nothing that says you have to go and change them. You can keep the old model, prevent changes to it via PDM permissions and require that people use the 'new and improved' models moving forward. 'Fix' the old stuff when you can.

bnemec wrote: ↑Thu May 27, 2021 3:13 pm I had to dig back in my notes now to see where we were with toolbox. At @JSculley mentioned, toolbox is not available in Standard which I had forgotten about and was helpful reminder because I wasn't looking back to before we purchased SW. It was a matter of chicken and egg. We couldn't get contextual examples of how we would set up TB and how it would work in our case with PDM and revising hardware and so on. Can't test it without buying it. Since we heard a lot of "hardware aren't revised" type comments we decided it wasn't for us. And, because there was nothing else in Pro or Prem that we needed we bought Standard.

Yeah if you don't have anything other than standard then TB just isn't an options. I've always wondered why they did that. I doubt people are going to upgrade to standard just to get the TB.

MJuric wrote: ↑Thu May 27, 2021 2:40 pm I spent a few minutes throwing your list into custom properties. I have zero experience using the Excel/PRT approach so have no idea how this compares to what you're doing. This is how it would work if you used the TB.

Any of those added properties can be used to create a new configuration, in descriptions etc etc. If you set up the TB to not create parts and only run on Configurations when you add the custom properties to configurations is automatically creates all the possible configurations in the part. When make selections it updates the config.

There are also several other options you can use in the TB as well, custom config names etc etc.

The graphics area to the right is also complete configurable. This allows you to create "Families" of parts which is alot easier than having everything in one file.

You can also export the entire thing into excel and do any other type of operation you want to create the database initially. For instance I export the information and used Excel to create all of our part numbers and descriptions based on a "Smart number" system I created and by concatenating fields made the description. I then uploaded that back into the TB.

ToolBox.gif

Thanks for taking time to do that. I watched over and over to keep up to the steps. It is interesting to see and brings back a bit of memories now.

Couple more questions:
- Is there anything preventing the user from using a part that is not available? as in not set up with a part number.
- If every possibility is generated at day one, how does an admin type user set the part number for that config once the part is actually available to use?
- you mentioned "When make selections it updates the config" I'm assuming that means the file cannot be in the vault? I'm not sure how this works for file references in PDM,
- Can I get a where used of a specific part number?

bnemec wrote: ↑Thu May 27, 2021 4:17 pm Thanks for taking time to do that. I watched over and over to keep up to the steps. It is interesting to see and brings back a bit of memories now.

Couple more questions:
- Is there anything preventing the user from using a part that is not available? as in not set up with a part number.

The way I have it set up if the part does not exist in the TB you can't get it. You can set it up so "Custom conFigs" are available although I have never tried to do that.

bnemec wrote: ↑Thu May 27, 2021 4:17 pm - If every possibility is generated at day one, how does an admin type user set the part number for that config once the part is actually available to use?

If you're setting a part number sequentially I'd suspect that you could do it with allowing "Custom Configs" but as above I have not tried that. What I did was create a smart number and apply that to every fastener in the TB. This was all done offline in Excel. This way a Unique part number was created for each part. Without having a better grasp of exactly how you are applying part numbers it's hard to say how'd you do it in TB.

Here is a screen shot of out TB. the noted column was generated in Excel. As it's smart number it's a combination of fastener features. In essence the admin would never have to set a part number once this was in place assuming your downstream systems could deal with that. You could also keep all your existing numbers as well but those would have to be manually entered in that field.

bnemec wrote: ↑Thu May 27, 2021 4:17 pm - you mentioned "When make selections it updates the config" I'm assuming that means the file cannot be in the vault? I'm not sure how this works for file references in PDM,

The file can be in the vault. There's a couple ways to set up the TB.

The user has to have write access to the TB part in order to be able to create configurations in the part. To be honest I'm not entirely sure what magic takes place for this to happen but the easy way is to just check the part into the vault.

When you use TB it pulls write access. Multiple people can do this at the same time...again no idea how this works. The dangerous part of this is that anyone can actually just check out the model and screw it up as well.

There is a way to set up the TB so that you can limit access to the model. Essentially you set up the TB as a specific user that has access to the TB models. When someone opens TB they indirectly become that user and are given read/write access to the model so they can do config changes. However no one can modify the TB models unless they actually are logged in as that TB user sign in. This essentially becomes an Admin log in that allows everyone to log in as admin but only under the controlled conditions of the TB.

bnemec wrote: ↑Thu May 27, 2021 4:17 pm - Can I get a where used of a specific part number?

This one I don't have an answer to. We don't do much with "Where used" in the PDM because that is in our ERP.

A quick google says you can do it but I'm not sure if that only applies to the "Create part" method of using the TB or all options. I just messed with ours real quick and I don't see any "Where used" data, but again I'm not real familiar with that so it may be there somewhere

as others said, in my opinion ToolBox is too limited.

it can be great for people who begin with SW, and doesn't know enough with PRT-Excel (configs).

but if you know enough how to use PRT-Excel, you can go far beyond, and faster, than the "Toolbox".

why having a "Library" with splitted Library-workflow ? some PRT-Excel, some Toolbox
it's easier to have only one Library-workflow (PRT-Excel).

plus, it's easy to add into PRT-Excel : auto-size, auto-mate, or publisher-panel
these features aren't exclusivity of the "Toolbox"

Just as a follow up incase anyone cares;
We've decided to backpedal on the configured hardware files. We are working our plan that attempts to break out the many parts in the configured files into individual part files with only the Default config. This is going to cost us a lot of labor but after discussions here and with our VAR as well as internally we believe that it's better to fix it now and leave configured hardware alone or it will likely cost us much more in the long run.

bnemec wrote: ↑Thu Jun 24, 2021 9:18 am Just as a follow up incase anyone cares;
We've decided to backpedal on the configured hardware files. We are working our plan that attempts to break out the many parts in the configured files into individual part files with only the Default config. This is going to cost us a lot of labor but after discussions here and with our VAR as well as internally we believe that it's better to fix it now and leave configured hardware alone or it will likely cost us much more in the long run.

So you're going to have a library with a model for every fastener?

MJuric wrote: ↑Thu Jun 24, 2021 9:40 am So you're going to have a library with a model for every fastener?

no and yes. No library, every fastener gets a file (serial number name with all the rest of the parts) and each one had our company's part number on data card.

I've only been a couple other places that use CAD like this and neither of them were at all like what we do here. I'm learning that as far as CAD and PDM conversations go our entire data set is "Standard parts library" either that or we don't have any standard parts.

@bnemec I would put these in a library for the engineers to easily use. Even if you separate them out however for performance displaying the library you may need more folders since there would be so many files.

Here is ours....not just fasteners.
_
They are all configurations based and fastener families (one model file), separate files by fastener type, head style, slot, material, finish. So one file contains configurations that just represent size, thread, and length. -
We create all standard sizes, and then apply part numbers as we go. This allows engineers to use sizes we don't stock when prototyping. Then they can add a new part number on an ECO if needed. -
Drag from library and pick by description while seeing if existing ones have a part number. Since the configurations are not named by part number, we put the part number in the configuration's 'Description' box.

bnemec wrote: ↑Thu Jun 24, 2021 9:18 am Just as a follow up incase anyone cares;
We've decided to backpedal on the configured hardware files. We are working our plan that attempts to break out the many parts in the configured files into individual part files with only the Default config. This is going to cost us a lot of labor but after discussions here and with our VAR as well as internally we believe that it's better to fix it now and leave configured hardware alone or it will likely cost us much more in the long run.

Hey @mike miller and @Jaylin Hochstetler,
I know you guys are demoing data management software.
You guys may want to have a look at this post because I believe this is one of the requirements for DDM. So, if you've got configurations DDM treats them as "files" in their DB. It's all tradeoffs and a comparison of how DDM handles this vs. that Quick Start package from Siemens may be a good idea.

mattpeneguy wrote: ↑Fri Jun 25, 2021 6:01 pm Hey @mike miller and @Jaylin Hochstetler,
I know you guys are demoing data management software.
You guys may want to have a look at this post because I believe this is one of the requirements for DDM. So, if you've got configurations DDM treats them as "files" in their DB. It's all tradeoffs and a comparison of how DDM handles this vs. that Quick Start package from Siemens may be a good idea.

That's interesting. Solidworks PDM Pro (Conisio) tracks configurations but not as separate files.

The problem we're having is configurations of pc parts wrecks where used searches. Mostly due to various versions of the file being used all over the place and to select a specific config the user must first select a specific version.

We are learning that in our case and with PDM it really is best to keep a 1:1 relation of file to part number. Configurations for various part numbers in one file being 1:n. We intend to use configs of assemblies that are used in various positions (top, mid, bottom for example). In the past we've had extra (duplicate) assembly files for those positions which is n:1 and it just makes a lot of extra work maintaining those models.

bnemec wrote: ↑Fri Jun 25, 2021 6:19 pm The problem we're having is configurations of pc parts wrecks where used searches. Mostly due to various versions of the file being used all over the place and to select a specific config the user must first select a specific version.

Not that it helps you now, but check the 2022 beta what's new. All I can say is 'finally'.

jcapriotti wrote: ↑Sat Jun 26, 2021 3:10 am Not that it helps you now, but check the 2022 beta what's new. All I can say is 'finally'.

Unless we ditch SW and go back to Edge we'll have to update to 2022, I don't want to go out more than three years and we're on 2019 so once SP4, or 5 (or 5.1 ) is out we'll be biting that bullet. Will be nice to have some things to show for the cost of updating.

bnemec wrote: ↑Sat Jun 26, 2021 3:35 pm Unless we ditch SW and go back to Edge we'll have to update to 2022, I don't want to go out more than three years and we're on 2019 so once SP4, or 5 (or 5.1 ) is out we'll be biting that bullet. Will be nice to have some things to show for the cost of updating.

The updates are still thin IMO for what we pay. Our PDM annual maintenance is as much as SolidWorks but the updates are few. still waiting on some sort of "Get Latest Released".

jcapriotti wrote: ↑Sun Jun 27, 2021 12:16 am The updates are still thin IMO for what we pay. Our PDM annual maintenance is as much as SolidWorks but the updates are few. still waiting on some sort of "Get Latest Released".

I cannot argue with that, but we've only used one version.

"Cost of updating" I didn't mean maintenance. I'm still trying to get a number together for what it will cost to just implement the update. People here were talking about updating to 2021, even the boss. While trying to research all that was really needed, the cost of testing the new release is insane. They (VAR, Solidworks, etc) can put "test your system" in one bullet point on the update check list; but a full test case in our system would take a team of three a week. That's after the time it will take me to get new SQL and Archive servers all installed and running. It's a tough pill to swallow and I cannot imagine that some do it every year; unless they don't test and and if there's a problem just let the fecal matter hit the rotary impeller.

As I've been reading threads from over the past almost 3 years and the stories of updates that cost the company $$$ I read many "Well didn't you test that?" comments or the user saying the VAR gave them that line. Based on those scenarios I'm trying to put test cases together, but actually being able to work those test cases might wind up costing more than the potential failure(s). What a predicament to be in, considering we're using "The greatest software in the world."

I was told early on to avoid toolbox, and I'm glad I did. I'm not sure what the relationship is between the two, but SW has issues with something as simple as the hole wizard. No way I would trust toolbox.

(Below is a gif.)

SPerman wrote: ↑Mon Jun 28, 2021 3:43 pm I was told early on to avoid toolbox, and I'm glad I did. I'm not sure what the relationship is between the two, but SW has issues with something as simple as the hole wizard. No way I would trust toolbox.

(Below is a gif.)

HoleWizard.gif

I've never seen anything like that since I started using hole wizard and TB, about five years now. That either has to be an error in the database and would be repeatable and all 1/4-20 would be that way or more likely someone manually renamed the feature breaking the link to the TB size.

If every 1/4-20 you place does this then it's a DB issue and SW needs to fix it. What version? Does it repeat?

bnemec wrote: ↑Mon Jun 28, 2021 9:47 am I cannot argue with that, but we've only used one version.

"Cost of updating" I didn't mean maintenance. I'm still trying to get a number together for what it will cost to just implement the update. People here were talking about updating to 2021, even the boss. While trying to research all that was really needed, the cost of testing the new release is insane. They (VAR, Solidworks, etc.) can put "test your system" in one bullet point on the update check list; but a full test case in our system would take a team of three a week. That's after the time it will take me to get new SQL and Archive servers all installed and running. It's a tough pill to swallow and I cannot imagine that some do it every year; unless they don't test and and if there's a problem just let the fecal matter hit the rotary impeller.

As I've been reading threads from over the past almost 3 years and the stories of updates that cost the company $$$ I read many "Well didn't you test that?" comments or the user saying the VAR gave them that line. Based on those scenarios I'm trying to put test cases together, but actually being able to work those test cases might wind up costing more than the potential failure(s). What a predicament to be in, considering we're using "The greatest software in the world."

In your situation I can see it would be tough, correct me but aren't you splitting your time as PDM admin and designing?

We have a production system with 4 servers (1 SQL and 3 replication). We have two development/test systems. I have one full time programmer for PDM/Solidworks custom apps and another programmer to borrow for some tasks and factory automation, plus a few power users I can bring in if needed. Generally we begin testing new Solidworks and PDM versions around SP2 in February for a planned rollout to sp4 around July.

You really need a full time test system and development system. Test cases are critical to a successful rollout. It's expensive but then again, so is waiting between too many releases as the amount of problems can multiple. Rolling out a broken system is worse, and not to mention stressful if you have to go before management. Because of Windchill and compatibility issues we had to wait to upgrade. We went from PDM 2017 to 2020. Lots of little issues. The search changes in 2018/19 broke most of our search cards. Next jump will probably be 2022, again because we can't update SolidWorks until our global company updates Windchill. Now you want to talk expensive.........I wish I had 10% of our Windchill budget.

jcapriotti wrote: ↑Mon Jun 28, 2021 6:18 pm In your situation I can see it would be tough, correct me but aren't you splitting your time as PDM admin and designing?

That was the plan but I'm still 100% PDM and CAD Admin. Fortunately there are a couple of very good users who are a huge help with the CAD side as I'm just not using it as much as they are. PDM is where my time has been going.

We have a production system with 4 servers (1 SQL and 3 replication). We have two development/test systems. I have one full time programmer for PDM/Solidworks custom apps and another programmer to borrow for some tasks and factory automation, plus a few power users I can bring in if needed.

I'm also the one and only API programmer, been trying to get another one hired.

Generally we begin testing new Solidworks and PDM versions around SP2 in February for a planned rollout to sp4 around July.

Are you kidding me?!?! Any idea of total labor hours dedicated to this?

You really need a full time test system and development system. Test cases are critical to a successful rollout. It's expensive but then again, so is waiting between too many releases as the amount of problems can multiple. Rolling out a broken system is worse, and not to mention stressful if you have to go before management. Because of Windchill and compatibility issues we had to wait to upgrade. We went from PDM 2017 to 2020. Lots of little issues. The search changes in 2018/19 broke most of our search cards. Next jump will probably be 2022, again because we can't update SolidWorks until our global company updates Windchill. Now you want to talk expensive.........I wish I had 10% of our Windchill budget.

bnemec wrote: ↑Mon Jun 28, 2021 6:29 pm Are you kidding me?!?! Any idea of total labor hours dedicated to this?

Lol....sorry, that does sound scary. I start testing early so I can find bugs, report them, and get them fixed before rollout. We support a number of applications so our time is split will many things.

PDM testing is probably about a week of testing in a normal year. Here's a few items this involves (guestimation in a normal year):

• Testing all search cards for expected results (4 hours)
• Testing all workflows (40 hours)
• Testing all add-ins and custom applications (40 hours...maybe more)
• Testing connected systems input/output (8 hours)
• Test server upgrades and client upgrade (8)
• Test database rollback and restore (4 hours)

There is more obviously and some of it is based on what changed in the new version. I test functions that changed more heavily than areas that didn't.

I think I spend more time getting our install package built and tested than actually testing PDM but we don't have IT support to do automated rollouts so we script it and let the users kick it off. At least it feels like it.

MJuric wrote: ↑Mon Jun 28, 2021 5:01 pm I've never seen anything like that since I started using hole wizard and TB, about five years now. That either has to be an error in the database and would be repeatable and all 1/4-20 would be that way or more likely someone manually renamed the feature breaking the link to the TB size.

If every 1/4-20 you place does this then it's a DB issue and SW needs to fix it. What version? Does it repeat?

It is just another one of those solidworks "features" that we all experience.

I opened the part this morning, and the feature is now labeled 1-16, even though it is still creating the proper 1/4-20 hole. My best guess is that my hole wizard database is corrupt. It's a database managed by solidworks, of course it will eventually become corrupt.

SPerman wrote: ↑Tue Jun 29, 2021 8:17 am It is just another one of those solidworks "features" that we all experience.

I opened the part this morning, and the feature is now labeled 1-16, even though it is still creating the proper 1/4-20 hole. My best guess is that my hole wizard database is corrupt. It's a database managed by solidworks, of course it will eventually become corrupt.

Yeah corrupt DB is definitely an issue with TB. I made a back up time I futzed with it because more than once it just had a complete meltdown.