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Attached are two files. They are copies of the same file. I included both because I wanted to check two conditions and I do not know if the actions of one effect the other.

This part was created using Driveworks Express. The issue I'm running into surrounds the marking of the holes.

Snapshot of the original The lettering is created via an array, custom property and varying the instance. When I run driveworks everything works fine, no errors. However for some reason the varying array does not work. New part.
Originally I was thinking it was an issue with the custom property not coming across, or something else. Everything seems to duplicate fine.

I tried to "Re-link" the text to the custom property and nothing happened so I went on looking for other issues. I continued to futz around and later tried to relink again and this time it worked and corrected not just the vertical text array but both vertical and horizontal arrays despite them being linked to two different custom properties.

So I went thru this exercise again, and same thing, didn't work. I finally figured out that if I went into FILE>PROPERTIES then existed and THEN relink it to the custom property...it then worked....which makes zero sense to me.

So if you have the time or the patience can you try the following.

1) first open one of the files and see if for some reason, for you, it magically updates properly. I'm on 2018 and maybe this is a "Fixed bug"
2) if it does not update please open the sketch and try relinking it to the custom property...see if that updates.
3) if not close that file and open the other one (To isolate the issue). Go to FILE>PROPERTIES. Don't do anything just leave it open for a second. Then repeat step two and then see if it updates. This is the only thing that will update it for me.

Sorry so complex but I spent probably 20 minutes trying to figure this out and it makes no sense to me.

Thanks

I opened the file in SW 2019. It has the "1" by all the holes when I open. If I do a rebuilt I get this:
Selecting File/Properties and hitting OK, then doing a rebuilt gets this:
The odd part is it rebuilds on opening, so why it changes between the opening rebuild and the next confuses me.

I get the same behavior in SolidWorks 2020.

EDIT - I re-read the original post and saw that File Properties was just opened, OK wasn't clicked. I tried again with hitting cancel after File/Properties. I rebuild after that and the text is fixed.

CarrieIves wrote: ↑Wed May 05, 2021 5:52 pm I opened the file in SW 2019. It has the "1" by all the holes when I open. If I do a rebuilt I get this:

image.png

Selecting File/Properties and hitting OK, then doing a rebuilt gets this:

image.png

The odd part is it rebuilds on opening, so why it changes between the opening rebuild and the next confuses me.

I get the same behavior in SolidWorks 2020.

EDIT - I re-read the original post and saw that File Properties was just opened, OK wasn't clicked. I tried again with hitting cancel after File/Properties. I rebuild after that and the text is fixed.

Great, thanks.

Looks like another SW bug. I will send it into my VAR and see what happens for them. Now that I figured out how to fix it, not that big of a deal but every one using my driveworks model will also have to "Known how to fix it". Fun, work instructions on how to get Solidworks to work...

Thanks again

It's the file name change. Just rename the file and open and the array all goes to "1". Rename it back it evaluates correctly.

I'm guessing this is because the filename is stored in the custom property syntax. Apparently you have to open the custom properties and "Ok" it and it updates whatever is causing the issue.

jcapriotti wrote: ↑Sat May 08, 2021 11:27 am It's the file name change. Just rename the file and open and the array all goes to "1". Rename it back it evaluates correctly.

I'm guessing this is because the filename is stored in the custom property syntax. Apparently you have to open the custom properties and "Ok" it and it updates whatever is causing the issue.

Yes, that is what I eventually stumbled to as well. I've done this several times and opening the Properties and "OK" seems to fix it in every case. Not a big deal I suppose, just not what one would expect to happen....but I guess I should expect it because expecting the unexpected is probably the norm for SW.

Interesting way to handle this but you're in the "red" area of pushing the software to the limits of what it's designed to do. I wouldn't be surprised to see this get broken in the future if they change something.

Years back before you could "Configure" equation Global Variables, we "cheated" the system by linking a dimension to the Global variable. I could then "configure" the dimension. This worked great until they "enhanced" the equations and tried to remove the linking function. In the end, they added it back and fixed most of the issues, but it was never 100% stable like it was. We had to rework a number of models.

jcapriotti wrote: ↑Mon May 10, 2021 12:09 pm Interesting way to handle this but you're in the "red" area of pushing the software to the limits of what it's designed to do. I wouldn't be surprised to see this get broken in the future if they change something.

Years back before you could "Configure" equation Global Variables, we "cheated" the system by linking a dimension to the Global variable. I could then "configure" the dimension. This worked great until they "enhanced" the equations and tried to remove the linking function. In the end, they added it back and fixed most of the issues, but it was never 100% stable like it was. We had to rework a number of models.

I think a good portion of what I'm currently working on is "In the red" for the software. But still the gains to be had here are significant even assuming some of it breaks in the future. Most of it is rather easily fixable after the Driveworks model is created as well. One of the big gains here is some level of uniformity. The other day I found ~15 models and drawings of parts we use regularly. Turns out most of them were duplicates or parts that we simply don't need and should have never been made in the first place. I've knocked those 15 parts down to 4, and those four will be the only ones available in my Driveworks model . If we need a "Special" it will be an entirely different model and it will never be included in the driveworks assembly.

Full Driveworks or Express? I would love to get my hands on the full product as I love messing with this kind of software but our company went a different direction for configuring.

jcapriotti wrote: ↑Mon May 10, 2021 1:25 pm Full Driveworks or Express? I would love to get my hands on the full product as I love messing with this kind of software but our company went a different direction for configuring.

Just Express, at the moment. If I can show enough advantage to using Driveworks I might be able to get them to spring for Solo. That being said I have only found the following things to be a PIA by using Express.

1) No variables. This becomes exceedingly painful when you end up nesting several things.
2) No Hole wizard functionality. Can't change an M6 to M8 and so on
3) Can't dictate where the files are created. All the files are created in the same directory as the original files. This obviously gets messy and complicated. I always end up saving the created files somewhere and then go into the original directory and deleting them.
4) Can only change dimensions in a single configuration.

All of the above, save the hole wizard issue, have painful work arounds.
1) Variables are replaced with the original formulas. You just end up with a painfully large formula. So far I've not hit character limitation there but I'm sure there is one.
3) Files are dealt with as above
4) in many cases you can create custom properties that are linked to the dimension and are "This configuration only". You can then link that custom property to something in driveworks and control that. Two steps instead of one but it works. I did this recently with a part that I had the part and the casting in. Any place where the casting feature and the finished part feature were the same I made two custom properties and drove those in Driveworks.

All in all the Express product is pretty powerful but I think if I were doing any more complex assemblies it would be ridiculously painful.

Thanks for sharing such a convenient number sequencing method. But for some reason, it doesn't work in SW2023 SP2.1.

All the pattern array feature shows the same property content, even its linked dimension DOES vary in different array entities.

I even tried to make a global variable linked to that dimension, and make a property linked to that global variable, but the text still refuse to change.

Attached is a combined picture that shows my sketch, text in sketch, custom property, and feature array result. I did the awkward "Open property" and exited by clicking "Cancel", re-linked the "Custom Property" in the text that you shared here, but all the results are the same:

All texts remains "1", even an included indicating rectangle does vary in length correctly.

For the sldprt files that MJuric shared here and in another post, they still show all as "1" once I execute a rebuild. None of them work in the SW version I am using.

I guess there is something prevents the Custom Property from updating itself within a Pattern Feature, but I spend almost an afternoon just trying to figure out in Options without any success, so I come up for asking help and hope someone might shed me a light...

Any thought would be appreciated.

I have not looked inside the files, probably unrelated to your work, but be aware that since 2019 (iirc) the custom property structure changed and since 2022 there is a command that force the upgrade of custom properties in legacy files.

I had a macro that did not work until I forced the properties upgrade.
in our data we also had some incident with welding cutlists properties that linked to a different file by their own and were beyond repair.

be careful before throwing additional money to SW as the product could not work as advertised...

Hi, just come back to make an update to say that there is a more straight forward way to this sequencing workaround.
So simply copy the dimension's full name and double quote it in your text window, instead of setting it in custom property and indirectly assigning it in text window, it magically solve the problem.

I did some search after and found there was already someone did the same. So here is the link for anyone who is still looking for it:
https://www.beacon-india.com/incrementa ... olidworks/

IDONTEXIST wrote: ↑Thu Oct 05, 2023 3:27 am Hi, just come back to make an update to say that there is a more straight forward way to this sequencing workaround.
So simply copy the dimension's full name and double quote it in your text window, instead of setting it in custom property and indirectly assigning it in text window, it magically solve the problem.

I did some search after and found there was already someone did the same. So here is the link for anyone who is still looking for it:
https://www.beacon-india.com/incrementa ... olidworks/

I did not know that you could do this!

Thank you for this post!!