Multiple Drawings pointing to the same Assembly

[jforsyth]

We are using CREO 3.0, M030

We need to create multple drawings that are linked to the same assembly.

Each drawing will be saved as a PDF and combined to make a single PDF.

Our Assembly has the file name "AAXXXXX"

The first drawing that is linked to the assembly will have a file name "BBXXXXX"

The second drawing will have the file name "BBXXXXX-101"

The third drawing will ahve the file name "BBXXXXX-102" and so forth.

We need the title block text on all drawings to read "BBXXXXX"

When I use the system parameter "&dwg_name" the first drawing is correct, but the subsequent drawings will show "BBXXXXX-101, BBXXXXX-102" and so forth.  I want all of the drawings to have the same title block text.

Looking throught he PTC Community post I have found and tried the following relations.  In preparation I ahve creted the drawing parramters ACTUAL_LENGTH, display_length,and drawing_no.

Here are the relations:

Relation 1

ACTUAL_LENGTH = STRING_LENGTH(dwg_name)
display_length = ACTUAL_LENGTH
if (ACTUAL_LENGTH > 7)
display_length = 7
else
display_length = STRING_LENGTH(dwg_name)
endif
display_name = EXTRACT(dwg_name, 1, display_length)

Relation 2

drawing_no = extract(dwg_name, 1, (search(dwg_name, "-101")-1))

For this relation I adjusted the "-101" to match the different drawing firl names acccordingly.

When I try either of these relations I keep getting an error stating that dwg_name is an invalid symbol.

What am I doing wrong?

[BenLoosli]

You have to use &dwg_name, not dwg_name.

That said, it is a system drawing parameter and you cannot use it like rel_model_name and truncate its length.

Why not just create multiple sheets in a single drawing file? They can all use the sheet 1 format.

[jforsyth]

Ben,

Thanks for your quick reply.

We typically have drawings with 50 sheets and more.  The response time is not acceptable.  It sometimes takes 5 minutes to change sheets.

Additionally, by dividing the drawing up into different drawings, we can have different drafters work on different drawings at the same time.

We have looked at different methods to improve the performance of our drawings with little luck.

We have also brought in a PTC vAR for assistance tand they reccommend this approach.

[TomU]

You should be able to do this with relations inside a single cell repeat region.  When REL_MODEL_NAME is used inside these relations it will refer to the drawing itself, not the model.  Simply search for the dash and then truncate everything after it.  Let me know if you need to see an example.

[jforsyth]

TomU,

Thanks for your quick reply.

I will take a look at your suggestion and see if I need further examples.

I will respond to this post after I try your suggestion.

[TomU]

This may help:

https://community.ptc.com/t5/Detailing-MBD-MBE/amp-model-name/m-p/607610/highlight/true#M27668

[MartinHanak]

Hi,

what about this ...

• in assembly relations get assembly name, replace its first two AA with BB and put the result into DRAWING_NAME parameter
• in drawing show DRAWING_NAME parameter instead of DWG_NAME system parameter

[jforsyth]

Martin,

I have not had any luck with the other suggestions.

Can you please send me an example on how to replace the AA withthe BB from the rel_model_name?

[MartinHanak · Accepted solution]

Hi,

in assembly define following relation

drawing_name="BB"+extract(rel_model_name, 3, string_length(rel_model_name)-2)