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Adding "general" notes to a drawing format.

JoeFrancz
1-Newbie

Adding "general" notes to a drawing format.

I am sure this is a simple one but I am spinning my wheels on how to do this. I would like to add a general note section(see example below) to the drawing formats so when the user creates a drawing they are able to edit these notes or add to them in the drawing. I tried adding an annotation feature to the start part and then placed the callout in the format (¬e) and when that format is used to create a drawing the note doesn't populate. I am trying to make this simple for the users so they don't have to create a NOTE, from file in drawing mode each time a drawing is created.


NOTES


1. BREAK ALL SHARP EDGES


2.


3.


Thanks for the help


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8 REPLIES 8

We handle this by having these types of items on the drawing that is
associated to our start part. The format is static and while it handles
data being entered into the tables well, notes are assumed to be part of
the format and, as you have seen, cannot be edited or moved.
Bob Frindt
Sr. Designer
Parker Hannifin Corporation
Parker Aerospace
Gas Turbine Fuel Systems Division
8940 Tyler Boulevard
Mentor, OH 44060 USA
direct (440) 266-2359

If I have any text that the users need to alter on my formats, I put it in a table.
If you add the text into a table on the format it can be edited after the format is added to the drawing.
A normal note on a format cannot be altered after it's added to a drawing.

Regards
Sarah Ford
CAD Designer
Westwind Air Bearings
Tel. 01202 627236

The way that we do this is with a mapkey that creates a note, no leader,
and then loads a text file that contains the wording that we the note to
say.



The nice thing about this is that we can add these notes to drawings
quickly and easily, and they are full NOTES that users can modify to add
or take away from. We have about 10 standard notes that we use in various
combinations on drawings. This also saves us from having 10 different
format types for all of these different types of drawings. This way, if a
drawing were to change type for example, you can simply delete the notes,
and reapply the correct notes, and leave the format alone.


We have these Items in the title block on the format. The entries come from the parameters within the model. These are part of a longer list of parameter items that are in our start parts. When the user creates a model, assembly/part, the entries are editable within the parameter file. When they start the drawing all the fields on the format are populated accordingly.


Parameters:


BREAK_SHARP_EDGES_FROM


BREAK_SHARP_EDGES_TO


In the Format


&BREAK_SHARP_EDGES_FROM


&BREAK_SHARP_EDGES_TO



Hope this helps.


Ilene Harris
Sr. Designer / Cad Administrator


Pacific Scientific HTL
1800 Highland Ave.
Duarte CA 91010
Tel: +1 (626) 434 1161
Fax: +1 (626) 359 7013
ilene.harris@meggitt.com
www.meggitt.com

jstone
4-Participant
(To:JoeFrancz)

We have all drawing general notes as symbols. They can be edited by using format/symbol gallery. Also variable text can be used to pick common notations.
Thanks,
jef

You want to add the notes to a drawing template, not the format.

You should look at my ProE Admin 101 talk I gave at PTC User in 2010



In Reply to Joe francz:



I am sure this is a simple one but I am spinning my wheels on how to do this. I would like to add a general note section(see example below) to the drawing formats so when the user creates a drawing they are able to edit these notes or add to them in the drawing. I tried adding an annotation feature to the start part and then placed the callout in the format (¬e) and when that format is used to create a drawing the note doesn't populate. I am trying to make this simple for the users so they don't have to create a NOTE, from file in drawing mode each time a drawing is created.


NOTES


1. BREAK ALL SHARP EDGES


2.


3.


Thanks for the help




Hi Joe...


You definitely want to add your notes to a drawing template. Templates give you the ability to add notes, symbols, and other annotations to each drawing as it's created. Davig Haigh's presentation probably covers this in depth. A drawing template is different than a format. Think of the format as just the drawing frame with relevant intelligent text you'd expect to see in a format (title block, rev block, border, perhaps a BOM, etc). A drawing template is much different.


Let's say you needed to make a series of injection molded plastic parts. All of these parts have similar notes. Let's say you also need to make a series of sheet metal parts with another set of notes custom to those sheet metal parts. Going further, assume you also have a series of machined parts with yet another set of custom notes and even some special symbols for part marking. In this situation, templates are your best friend.


You can have one template for the injection molded parts, one for sheetmetal, and a third for machine components. All three templates can use the exact same ANSI-D sized format (with title block, etc). Yet each template can contain different notes, symbols, and other annotations specific to the parts they'll be used to detail. Your sheetmetal template may have notes regarding bend allowance while your plastic template may contain a note indicating the acceptable shrinkage range.


You can actually turn any drawing into a template. Let's say you've made a drawing of a cut piece of pipe. You can use that drawing as a template to create OTHER drawings of cut pipe re-using the notes, symbols, views, tables and related annotations and simply replacing the model.


Give David's presentation a look. If you have any questions afterward... please ask!


Thanks!


-Brian

Hi all,

My apologies if this has been asked before. Is anyone running Wildfire 2 with Windows 7? Looks like they're not compatible.

Thanks,
Stefan
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