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BDUB2012
Posts: 47
Registered: ‎03-14-2012
Message 1 of 12 (1,335 Views)

Prompted Entry

1335 Views, 11 Replies
04-13-2012 10:14 AM

It was suggested to me to make the revision and reference drawing fields in my titleblocks prompted entry and the fields that I want searchable to be iproperties. Is this the best way to set up titleblock info. The only time I see that you can edit prompted enties is when you use the template on a new drawing.

 

Thanks

*Expert Elite*
jtylerbc
Posts: 864
Registered: ‎09-01-2010
Message 2 of 12 (1,319 Views)

Re: Prompted Entry

04-13-2012 10:41 AM in reply to: BDUB2012

To edit the prompted entries, look in the Browser, on the sheet in question, and find your title block in the list.  If you click the + to expand the item under it, you should see an entry for your prompted text (Field Text).  Double-clicking it or right-clicking and picking "Edit Field Text" will allow you to edit the prompted text entries in the title block.

 

Also, I don't think I'd agree with the advice to make your revision a prompted entry.  If you follow the 1 drawing file, 1 sheet method, there is the Revision iProperty that you can use along with a drawing scope Revision History table.  If you put multiple drawings as seperate sheets into the same file, there is the Sheet Revision property that you can use with the sheet scope Revision HIstory table.  Seems odd to me to create your own Revision field, when two built-in possibilities already exist.

John Tyler
Inventor 2013
Windows 7 64 Bit
Active Contributor
BDUB2012
Posts: 47
Registered: ‎03-14-2012
Message 3 of 12 (1,313 Views)

Re: Prompted Entry

04-13-2012 11:01 AM in reply to: jtylerbc

OK, I find the text field. Please educate me on the one drawing file with one sheet method. I will have a master assembly with a dawing and then I will have sub-assemblies with drawings and I will also have parts with drawings. If I understood the one file one sheet better I guess I would then ask which method is better and what the pros and cons were. If you are referring to the revision table that can be inserted into your drawing, I would like to stay away from that if possible and the main reason for that is it can not be locked down and we have several people that would manifuplate it and save the file.

 

Thanks

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jtylerbc
Posts: 864
Registered: ‎09-01-2010
Message 4 of 12 (1,307 Views)

Re: Prompted Entry

04-13-2012 11:20 AM in reply to: BDUB2012

It's pretty literal.  Let's say you have an assembly drawing, and some subassembly drawings, and some individual parts.

 

If you use the one file / one sheet method, then that would be a seperate IDW file for each of those drawings.

 

If you use the same file / multiple sheets method, then you might have one IDW file, with multiple sheets for each of your drawings.

 

Personally, I prefer the one file / one sheet method, and I think that's the general consensus.  The reason would be largely related to memory management.  You're only loading data for the drawing that you want to work on, rather than loading pages and pages of irrelevant drawings when all you want to do is put a balloon on your assembly drawing or a dimension on one of your parts.

 

Some people prefer the multiple sheets method because it is fewer files to manage.  Desire to use it is often a side effect of long-term AutoCAD exposure.

 

My personal rule is that anything that is considered a seperate document (has its own drawing number) gets its own file.  If it is something like a specification sheet that is multiple pages which are part of the same document, I'll keep them in the same file on different sheets.

 

With regards to your revision issue - you can use either of the two properties I mentioned without having a history table on the drawing sheet.  The properties coordinate with the tables, but do not require them to be able to function.  That being said, I have trouble imagining how you could have drafters that you don't trust with a revision table, but would trust with a property or prompted text that can't really be locked down either.

John Tyler
Inventor 2013
Windows 7 64 Bit
Active Contributor
BDUB2012
Posts: 47
Registered: ‎03-14-2012
Message 5 of 12 (1,301 Views)

Re: Prompted Entry

04-13-2012 11:38 AM in reply to: jtylerbc

I want to apologize for the fact that I am a newbe and I am just trying to help our admin set things up so I am glad I found this website. I do not want to be a pain and appreciate everyones patience.

 

We will be using the one file one sheet method.

 

So with that said you, suggested the Revision iProperty that you can use along with a drawing scope Revision History table. I have played with the revision table a little and is the revision iproperty in that area or in the iproperties dialog. How do you have revision iproperty field filled out, not show the table on the drawing and get them to link to text in the titleblock.

 

Thanks

*Expert Elite*
jtylerbc
Posts: 864
Registered: ‎09-01-2010
Message 6 of 12 (1,289 Views)

Re: Prompted Entry

04-13-2012 12:02 PM in reply to: BDUB2012

You're not being a pain, that's largely what these boards are for.  I'm supposed to do support like this for Inventor users in my company, but we've been so slow about getting people up and running that I don't have many to help.  I use the boards to keep sharp for when we eventually do.  Also, it often turns out that when I'm helping people here, it reveals a better way I could be doing something myself.  Oddly enough, sometimes it's the newbiest of questions that end up revealing to me that I've been doing something really, really stupid for a long time without noticing.

 

The Revision Number iProperty exists in both places (table and iProperties dialog).  Think of it like this - the iProperty "Revision Number" is only the CURRENT value for the drawing revision.  The table shows both the current and previous values.  When adding rows to the table, be sure to understand the difference between adding "Rows" and adding "Revision Rows".  Adding just a Row gives you more text boxes to type in, but does not increase the revision level.  Adding a Revision Row moves you up to the next revision level (1 to 2, A to B, etc).  The only difference in operation between having and not having the table is that you don't have the record of previous revisions, and instead only have the current value for the property (just like the way Part Number or Description fields work).

 

In your title block, you'll insert a piece of text, and use the dropdown menus in the text editor to select "Properties - Drawing", then insert the Revision Number property.  Take a look at the default "standard.idw" template that ships with Inventor as an example - the title block includes the same sort of reference to the Revision property.

John Tyler
Inventor 2013
Windows 7 64 Bit
Active Contributor
BDUB2012
Posts: 47
Registered: ‎03-14-2012
Message 7 of 12 (1,284 Views)

Re: Prompted Entry

04-13-2012 12:21 PM in reply to: jtylerbc

Your last entry seem to cover updated the drawing revision and that would be another question I have. Is the drawing revision controlled and changed with vault or is that drawing revision number changed by the drafter in the drawing itself when a revision is made.

 

I made the revision table part of my titleblock definition. Do you use the IV revision table and make it seperate from the titleblock.

 

Considering I made it part of my titleblock definition I have fields for rev number, rev desciption, drafter, checked and approved for six revision levels that I need to be able to fill out. Do I link these to iproperties, revision table entries of what is the best way to fill these fields out.

 

Thanks

*Expert Elite*
jtylerbc
Posts: 864
Registered: ‎09-01-2010
Message 8 of 12 (1,276 Views)

Re: Prompted Entry

04-13-2012 01:26 PM in reply to: BDUB2012

You'll need to talk to someone else about the Vault's involvement - I've never used it, so I don't know how it affects the situation (or even IF it affects it).  So obviously, in my case, the drawing revision is just manually changed by the drafter.  Adding a revision row to the Revision History table increases the revision level, updates the property, and therefore the title block that is also referencing it.  It also increases the revision level that the revision tags will show by default (though you can still manually change them to older revs if necessary).

 

We use the Revision History table.  Our AutoCAD drawings have an integrated title block/rev table, so for some consistency of appearance we put the revision table in Inventor drawings next to the title block.  If you use the revision table built into Inventor, it will take care of all of those revision-related fields (rev, drafter, checker, ect).  The columns in it are also customizable by editing an individual table, or by editing / creating revision table styles.  If you use the built-in table, you won't even need those fields in your title block.

 

You don't actually link your prompted text to an iProperty.  You insert the iProperty into the text box instead of the prompted text.  In the text editor, there are two dropdown menus (initially blank) labeled "Type" and "Property."  "Type" switches between different types of property lists (drawing properties, model properties, prompted entry, etc).  "Property" is used to pick a specific one from that list.  At the end of that row of menus is a button to insert the selected property in the text box.  These are the same menus you would have used to insert prompted text, you're just picking different things from them.

 

In the case of revisions, what happens is that the title block shows the value that is in the iProperty "Revision Number."  If you are using the table, then when you add a new revision row, the iProperty is updated, which then also updates the title block.

If you still have it, I'd suggest playing around a bit in a drawing created from the original "standard.idw" template.  Place a revision table (drawing scope).  Look at the table, the iProperty, and the title block, and note that they're all matching.  Double click the table, and click "Add Revision Row."  Click OK, and go look at the three items again - note that they still match.

 

I think you're making things harder on yourself than they have to be, by trying to build your own instead of using a built-in tool.  If you save the template with a revision table placed, it will be there when you start new drawings, just like the title block.  I'm not really seeing any advantage to the combined title/revision block.  It certainly isn't any more secure than the revision history - the drafter would just go to a different place to mess with the history data.

John Tyler
Inventor 2013
Windows 7 64 Bit
Active Contributor
BDUB2012
Posts: 47
Registered: ‎03-14-2012
Message 9 of 12 (1,269 Views)

Re: Prompted Entry

04-13-2012 02:23 PM in reply to: jtylerbc

I appreciate all the info and will play with it. The main thing I was talking about not trusting the drafter is not the information in the tables but the table itself. I wish the table could be locked so that you couldn't grab a corner and drag it or accidentally move the whole table.

 

Thanks.

*Expert Elite*
jdkriek
Posts: 528
Registered: ‎03-29-2007
Message 10 of 12 (1,246 Views)

Re: Prompted Entry

04-14-2012 07:14 PM in reply to: BDUB2012

A note on the revision system in Vault - we don't use it and I don't know many companies that do either. Simple fact is with that system you can never cancel a revision made or roll back to a previous revision. Instread we link the Revision property in Inventor to a custom property in Vault. When the drafter changes the revision in the drawing and checks it in, the linked property in vault shows the revision. You can add this to all existing files as well by the "add property" action in Vault if the property doesn't already exist.

 

Here's a few older blogs from Brian Schanen that still apply in later versions giving you the basics:

 

http://underthehood-autodesk.typepad.com/blog/2010/10/vault-tip-of-the-week-splicing-in-properties.h...

 

http://underthehood-autodesk.typepad.com/blog/2009/08/setting-up-user-defined-properties-with-vault-...

 

 

Jonathan D. Kriek

Autodesk Inventor Certified Expert
Microsoft Certified Application Developer
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