Parameter in config.pro

[TomaszKazubski]

Is it possible added parameter to config.pro, which value will be switch on in drawing (exactly in format.frm)?

For instance, in company without PDM users need change standard iso to others (on drawing).

They using main config.pro and it couldbe good soluion that admin will change value of parameter in config.pro and finaly in all users will be changed it automaticaly.

Maybe other possibility not exactly in config.pro?

[KenFarley]

Any such parameters we use in drawing format, particularly things like "Design By" or "Drawn By" and the like, are defined in the part or assembly. Logical, since the person doing the drawing for a part or assembly is often NOT the person who did the design. The method I use to get "defaults" for these parameters for the stuff I design is I have my own personal start parts and assemblies, with my name in the pertinent fields.

Another possible thing you could implement is to define a mapkey that will set the parameters of interest, so when someone is making a drawing they can quickly set the "Drawn By" or any other settings you need.

[TomaszKazubski]

Of course I know about automatic parameters from template, but as I told please imagine situations that company works with one global config.pro and templates and for instance administrator want change some parameters without changing this template.

He use only config.pro or other files conecting with templates, format (.frm) etc. and finaly users do not need modyficate separetly this files.

Only one admin make change, something like LAYOUT for SKELETONS and all users have the same parameters (DESIGN BY , DRAWN BY is switch on from enviroment variables or name machine).

[BenLoosli]

You can define parameters to pull data from a Restricted_Parameter.dat file in format cells. This will give the user a drop down list of values for parameters.

[FV]

did you try to use ModelCheck's "SpellChecker" utility with custom dictionary?

Custom dictionary file - it is where you could associate a text to be replaced with the new one. I don't know though if it would go into notes carried from formats.

Another option is to use a weblink ( or any free API's) to setup an action listener and subsequent DtlNote modifications 

[MartinHanak]

Hi,

format can contain:

• fixed text ... e.g. Version
• parameter callout ... &version

You cannot change fixed text in format from outside.

So admin must prepare different set of formats for every fixed text.

[TomaszKazubski]

So, it's mean that no other possibility for diffrent fixed text? Maybe config.sup or others file?

[MartinHanak]

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@TomaszKazubski wrote:

So, it's mean that no other possibility for diffrent fixed text? Maybe config.sup or others file?

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Hi,

simple answer = no.

Fixed text is saved inside .frm file. If you want to change it, you have to modify existing .frm file -OR- create new .frm file.

[rreifsnyder]

You can also setup table cells in the .frm file that will be able to be modified per drawing or to use the parameter callout.

[MartinHanak]

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@rreifsnyder wrote:

You can also setup table cells in the .frm file that will be able to be modified per drawing or to use the parameter callout.

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Hi,

yes, tables saved in .frm enable user to modify their cells in .drw, but:

• OP looks for possibility to automatically switch fixed text
• when you replace .frm in existing .drw and remove all tables then your modification is lost

[YaroslavSin]

In config.pro you can save a Mapkey to change parameter value. Admin can change this value. But user must start mapkey manually.

[BR84]

Hi Tom,

• in format creation you have to call parameter names like: &MODELED_BY, &MASS, &MODELED_BY, &CHECKED_BY, &DATE_OF_CREATION, you name it
• open template drawing - choose the above format (you will have to retype parameters callouts)
• when you create a new drawing with a newly created template drawing, and if those parameters are specified in the part/assembly, they will be taken from the part assembly and displayed on the drawing
• parameters can have multiple values - for tolerances we have coule of default values that can be selected when needed

A assume that by ISO you mean drawing size - A4, A3

each size requires its own format - you can change it in drawing - I have created mapkey to change formats - one button - A3, another button A0, or empty format size 10000 x 10000

regards

[Chris_Johnson]

If you have Windchill this is relatively easy. There are already a set of parameters that are created on the Creo document called PTC_WM_??? which have data such as the creator or the person who last modified it. It is in Windchill format, which you might need to change, in my case it would read "Chris Johnson (cjohnson:<organisation name>)". You can use relations to truncate that back to a username or the user's full name. 

If you don't have Windchill, then I'm not sure you can do this and other way than customisation with the JAVA, VB or C Object Toolkit APIs. Those are pretty tough to get started with, but quite well documented once you get started. I've created a couple of programs in the OTK JAVA Free API and it is really powerful. You could use Java to read a config file or read an environment variable (Java command System.getenv(username) should do it) and push the result to a Creo parameter. That's quite tough to do if you've never touched the API before, but pretty easy for someone who knows what they're doing. 

For a fixed value of a parameter, you can use modelcheck. You need to add an entry to the start file to add the parameter and value. E.g add the line: 

DRW_PARAMETER	ISO_STD STR EQ ISO1101:2017

When modelCheck runs with MU set to YES, it will update the model to add the parameter ISO_STD to your drawing and fill the value in as ISO1101:2017. 

You can use logic (i.e. IF X = some value then run this set of config), to choose which config to run. That's in the condition.mcc file. Check the help files out or the knowledgebase to get an idea of how to set up ModelCheck.