Skip to main content
R
rallen-21-Visitor
1-Visitor
November 12, 2014
Question

One drawing template for both Parts and Assemblies

  • November 12, 2014
  • 3 replies
  • 3835 views

Is there any way to create a single drawing template/format that can be used for both parts and assemblies? The main difference being the addition of a BOM table for an assembly.

 

Essentially, I want the template to recogonize if I'm pulling in an assembly and show the BOM table, and if it's a part, don't show the table. I was hoping the Drawing Program interface would give me similiar capabilities to Pro Program, such that I could set up a relation to turn features on/off. However, it doesn't appear to work that way.

 

Is this possible? Or am I stuck with using two templates?

 

Thanks for any and all help.

 

--


This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

3 replies

B
23-Emerald III
BenLoosli23-Emerald III
23-Emerald III
November 12, 2014

I use the drawing program to switch layers on and off depending on a parameter value. Not sure if it is smart enough to do it automatically. You could set up a parameter in your start parts that is read by the drawing program to turn on the BOM layer if the part loaded into the drawing is an assembly.

R
rallen-21-VisitorAuthor
1-Visitor
November 12, 2014

I actually tried something similiar to this, however it didn't seem to work.

Here's what I did:

1. Defined a State through Drawing Program that blanked the layer containing the BOM and called it Part.

2. Edited the program and inserted the following:

IF &MBR.TYPE == PART

SET STATE PART

ENDIF

It says there is an error in line one so I'm assuming it's having an issue with the &mbr.type parameter (I also tried asm.mbr.type). Is there another parameter that returns the part type? Or is my syntax just wrong?

Thanks again.

L
LukaszMazur16-Pearl
16-Pearl
November 13, 2014

There is no such system parameter as mbr.type, so that's probably why you're getting errors. There is asm.mbr.type which holds the information on type of every component used in assembly you put in the drawing and there is type, which is a system parameter for type of the active drawing model.

In your case I'd try to go with

IF &TYPE == PART and so on.

H
huggre1-Visitor
1-Visitor
November 19, 2014

Create a format with two sheets, one with a partslist and one without.

When creating a drawing based on this format the system will ask you to select the appropriate format sheet.

Hugo

T
23-Emerald IV
TomU23-Emerald IV
23-Emerald IV
November 19, 2014

One thing to keep in mind, if you have the BOM table on the format and then reapply the format (to change sheet sizes, etc.), the BOM table may be removed and then recreated (depending on the selection made on the "remove old tables" dialog). That means any balloons that have been created will be lost. For this reason I prefer to add the BOM table manually to assembly prints. That way no matter how the format is reapplied, it will never impact the BOM table. It's certainly easy enough to create a mapkey to automatically add the BOM table and even create the balloons.

Terms & ConditionsCookie settingsAccessibility statement