need a UDF or something to change drawings to dual dimensioning.

[B_Baker]

I am using Creo Parametric Release 9.0 and Datecode9.0.4.0

I have 3 groups in our company that use the same config.sup and config.pro.
All use the same drawing formats. One group want to use dual dimensioning. I am not willing to give them different drawings with different .dtl files.
Is there a way to create UDF or set a local config option that will allow them to use dual dimensioning without going thru all of the selections to set up dual dimensioning? i have the drawing .dtl file set up so that when they change to dual dimensioning, all other settings are ready to go.
Just looking to shorten the 9-10 clicks per drawing to change to dual dimensioning.

Here are the errors that I faced
no errors

[KenFarley]

Perhaps you could make a mapkey to execute all the settings needed. Put it in either of your "used by all" config files, and let the users know what the key is. Possible drawback would be a conflict with particular users' personal mapkeys.

[Chris3]

Yes, we have this. I created a mapkey that loads in a dtl file on top of the company dtl file to make these changes. I then made a button for it in the UI so all users need to do is click the button. Below is our mapkey:

!=================================================================
!== load Dual Dimension IN / mm
!=================================================================
mapkey loaddualinmmdtl @MAPKEY_LABELDual IN/mm;~ Command `ProCmdDrwSetup` ;\
mapkey(continued) ~ FocusOut `preferences` `InputOpt`;~ Activate `preferences` `Open`;\
mapkey(continued) ~ Trail `UI Desktop` `UI Desktop` `DLG_PREVIEW_POST` `file_open`;\
mapkey(continued) ~ Input `file_open` `Inputname` \
mapkey(continued) `Q:\\Folder\\Path\\dwg-setup_dual_dims_in_mm.dtl`;\
mapkey(continued) ~ Activate `file_open` `Inputname`;~ Activate `preferences` `ok`;\
mapkey(continued) ~ Activate `main_dlg_cur` `page_Annotate_control_btn` 1;

The dtl file looks like this:

decimal_marker PERIOD
default_tolerance_display_style STD_ASME
dim_tol_lead_trail_zeros SAME_AS_LEAD_TRAIL_ZEROS
dim_tol_trail_zero_max_places same_as_dim_tol
dim_trail_zero_max_places same_as_dim
dual_digits_diff -1
dual_dimensioning PRIMARY[SECONDARY]
dual_secondary_units MM
gtol_lead_trail_zeros SAME_AS_LEAD_TRAIL_ZEROS
gtol_secondary_value_precision ROUND
lead_trail_zeros std_english

We have one for mm/in as well

[B_Baker]

I couldn't get the UDF option in drawings.  Seems that it was only in the part file.  All configs are set except the switch to dual dimensioning.  Now looking at trying to set up a custom pick in the Ribbon.

[BenLoosli]

Your terminology is off!

A UDF is a User Defined Feature used to create features from a 'template sketch' (UDF). They only apply to modeling.

What you need is a mapkey to do the change in your active drawing.

Another option is to use a group config.pro in the users Home folder. I did this when I had multiple groups using the same network install of Creo. The loadpoint config files would load and then the one in the home directory, followed by the config.pro in the Start-In folder. I had a batch file that ran at Creo launch that would delete and copy my 'standard' group config.pro, so depending on which login option they choose, it would set up the proper drawing formats and Windchill system. While my system required multiple drawing templates, you could also do it so only the mapkey to set dual dimensioning is set for that one group.

[B_Baker · Accepted solution]

A maykey was created and pushed out thru the groups/added to the Quick Access Toolbar.