Tables sometimes don't update (Creo 8.0.12.0)

[JM_10432119]

This is an annoying fringe issue. But I have tables with notes (notes have two lines of string values) and sometimes when I update a string value the note doesn't update in the BOM automatically. Nor does it update when I update tables. It seems to only update when I go to modelling and make sure it's regenerated and go to annotations click on the note and look at the text in text editor and then update tables. 

Does anyone have any ideas how to fix this? Maybe next time it happens I'll check whether it prints the correct info and creo is just showing the old info.

[Srinivasan-Iyer]

From the Description, it appears that you are using a Repeat Region for the BOM Table. I presume that Notes are not part of the Model Parameters, but Comments inserted in the BOM Table outside of Repeat Region. If you wish to associate the Notes with the component, it is always a better practice to have them as a Parameter in the Model. That way the parameter can be included in the BOM Table. Would also help in MBD.

Hope my understanding is correct.

Regards

[JM_10432119]

BOM is repeat region and notes are parameters in the model.

[Srinivasan-Iyer]

Then the problem should not occur. It should come in as any other parameter. Creo has a liking for multiple Regens😁. Try Regen 2 or 3 times.

Alternative: Try clicking the icons in the order given below.

[MartinHanak]

Hi,

please upload Creo files for testing purposes. It is necessary to pack files into single zip file and upload this zip file.

[JM_10432119]

I've been fixing them and don't have an example right now.

[JM_10432119]

OK I have an example and cleaned it of company data. I'm using creo 8 as I said and in the BOM top right the second line should say "1" STR. FLG. 4" I.K.R. WELDED TO ITEM 3/2" but is missing the addition "WELDED TO ITEM 3/2". Also I changed the spec. to remove the second line and that didn't update. Regen and update tables doesn't update it. I did have relations but I deleted them, they indirectly impacted description before but I removed that parameter from the note and added "WELDED TO ITEM 3/2" to description2.

[MartinHanak]

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@JM_10432119 wrote:

OK I have an example and cleaned it of company data. I'm using creo 8 as I said and in the BOM top right the second line should say "1" STR. FLG. 4" I.K.R. WELDED TO ITEM 3/2" but is missing the addition "WELDED TO ITEM 3/2". Also I changed the spec. to remove the second line and that didn't update. Regen and update tables doesn't update it. I did have relations but I deleted them, they indirectly impacted description before but I removed that parameter from the note and added "WELDED TO ITEM 3/2" to description2.

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Hi,

I do not have Creo 8.0.12.0 installed. Instead of it I used Creo 12.4.2.0. When I open your drawing I can see:

In message window I can see:

Suggestion:

• set config.pro option ... SAVE_DISPLAY NO
• open drawing
• apply all update actions
• save drawing
• restart Creo and open saved drawing

I hope someone else with Creo 8.0.12.0 installed will test your drawing.

[JM_10432119]

That didn't work. Also that table you screenshotted is what I use to quickly change parameters in drafting. It always updates, The the string values (DESCRIPTION1, DESCRIPTION2) have there own cells. 

[MartinHanak]

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@JM_10432119 wrote:

That didn't work. Also that table you screenshotted is what I use to quickly change parameters in drafting. It always updates, The the string values (DESCRIPTION1, DESCRIPTION2) have there own cells. 

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Hi,

please specify what table is causing problems ... upload a picture and highlight it in it.

Note: I modified values of parameters DESCRIPTION1, DESCRIPTION2 in the part and then switched Creo to the drawing. Table located under bottom line of drawing frame was update automatically and new values we displayed.

[StephenW]

@JM_10432119 

I'm on Creo 8.

By chance, is this an older drawing originally? Maybe save-as?

I believe that you need to apply the Drawing option update_drawing all

This fixes known issues in older drawings. There is a list of specific drawing updates but the "all" options eliminates the need to go find the exact one.

This link is the "how to" apply these drawing option updates: https://www.ptc.com/en/support/article/CS137953

I always suggest trying this option but DON'T IMMEDIATELY SAVE. Check your drawing thoroughly just in case something is messed up and you can get back to the unmodified version.

I was also able to get it to display correctly in the drawing by doing a force regen in the model, either by dragging the insert mode up, dropping it just below the csys and then taking it back down. Or by using the model player to force the regen. But I think the real fix is the drawing update_drawing all option.

[JM_10432119]

It is a save-as from a drawing originally creo 2 with stuff added onto it and me adding automation into it. I added update_drawing all to the config.pro to no effect. Also I can't find that option in drawing properties maybe it's hidden or not available in creo 8.

But I feel closer to an answer could be some drawing option or I'll look into the model player.

[MartinHanak]

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@JM_10432119 wrote:

It is a save-as from a drawing originally creo 2 with stuff added onto it and me adding automation into it. I added update_drawing all to the config.pro to no effect. Also I can't find that option in drawing properties maybe it's hidden or not available in creo 8.

But I feel closer to an answer could be some drawing option or I'll look into the model player.

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Hi,

update_drawing all detail option is the special one. It must be added manually -AND-  and it disappears from the list when you close dialog box and update the drawing.

[StephenW · Accepted solution]

NOT config.pro option, drawing option. go to FILE - PREPARE - DRAWING PROPERTIES - DETAIL OPTIONS CHANGE - manually enter UPDATE_DRAWING ALL.

Being an older drawing, it has accumulated "errors" (for lack of a better word) that PTC has fixed BUT only with manual intervention (there is a config setting to make this automatic).  It's manual because it MAY cause unexpected/unintended changes that are not desired. PTC works to not make "unexpected" drawing changes automatic, its one of their things. Its a pain in these situations to manually have to do it, but unexpected changes can be catastrophic if they go un-noticed.

[StephenW]

If the parameters modified are used DIRECTLY in the repeat region, it should just update or at the very worst, an update tables should handle it.

IF the parameters modified are used in a RELATION to combine them in to a string that is then used in the repeat region, then a model regeneration would be required.

There are probably a million other scenarios that could affect this but this one is very common, in my opinion.

[Srinivasan-Iyer]

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@JM_10432119 wrote:

(notes have two lines of string values) 

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I am curious to know how you could create a value in two lines. I tried to do it but could not.

[StephenW]

I don't know how others do it, but we break up lines to different parameters and then, depending on where it is used, we will either use the individual parameters or a parameter driven by a relation to combine the lines.

It's mostly for the 3 lines of our title block description, that was the driving reason it was done, it comes in handy for other uses occassionally and if the lines were split up wisely, not always the case with some users.

[JM_10432119]

We do it a different way which I think can be faster for automating stuff because you can type words and parameters into notes. That way to get the same effect you'd have to type longer creo relations.
There's a parameter type of note and annotating in model space you can add note 0, 1, ... string values and other parameters can be used.