DRAWING REVISION UPDATES

[Anonymous]

Hi Guys,

Simple question. How do I change the revision in Inventor 2012 without the older revision tags updating?

My drawings are now rev E and I have one rev D tag pointing to a component. That rev D tag updates to rev E after I change the drawing revision. It must be linked somehow and I have no idea where the links is. I want to have 2 tags one rev D and one rev E.

[Anonymous · Accepted solution]

My best guess from the Help file:

"Revision tags indicate the revision for objects on the drawing sheet. The resource for the revision number displayed in the revision tag is the corresponding revision table. When you create a revision tag, it displays the revision number from the active row. To display another revision number, right-click the revision tag, and then select a revision number from the Tag list."

So after you update the revision you will have to go back to the older tags and update/correct them manually.

[cadman777]

Thanks for this info.

Too bad nothing works.

I found that the "Update Propert to Revision Number" button doesn't activate anything. And when you have to or more different rev no's in separate rev table rows, the program gets all confused and doesn't work at all in updating the REV iProperty. Basicall, that button is useless, and so is using multiple rev table rows.

I thought the days of  Autodesk shoddy programming were gone.

Guess I was wrong.

My solution:

Ignore STANDARD DRAFTING AND REVISION PRACTICE, and list in the rev table ONLY ONE revision (i.e., the most recent).

... Chris

[jtylerbc]

When you add a revision row to the table, and set it to the new one, old revision tags should not change.  Once you add a new Revision Row, the old tags stay tied to the previous one, and do not update.

You are most likely using the wrong "Add Row" button.  There is a button simply titled "Insert Row."  This is used when your revision requires multiple rows to explain.  Then there is a "Add Revision Row," which is what works with the property update you referred to.  I am fairly certain there's nothing wrong with what the software is doing, you're just using the wrong button.

[cadman777]

That's the ticket; worked good enough.

Tell me what the purpose of the "Update Revision" button is in the upper right corner of the dialogue box? It doesn't do anything that I can see.

I guess I have to take back what I said about "shoddy programming" ... maybe.

Let's call it "scattered GUI", since commands are not where you would expect them.

Again, thanks ... Chris

[jtylerbc]

"Scattered UI" I can agree with - I've seen this problem many times with many users (including myself when I first started with Inventor).  It seems the placement of the buttons makes it more natural to pick "Insert Row", so people just instinctively start setting it up wrong.

I think that button is just a toggle that turns the association between the table and the Revision Number iProperty on and off.  I've never really used it, so I could be wrong, but I think it's simply the equivalent of the property update check box  in the rev table creation.  In my opinion, if that's the case, it should always just be left on.  I can't really come up with a situation where I wouldn't want the iProperty updating when I add a revision to the table.

[Curtis_Waguespack]

Hi cadman777, 

If you're talking about the Update Property to Revision Number button, it does pretty much what it's title suggests; if selected it writes the value of the REV cell for the active row to the Revision Number iProperty (or the Sheet Revision property if that's the way the drawing is set up). If it is not selected the revision table changes exist only in the table and are not written back to the proproperties.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[cadman777]

Curtis,

I figured that's what supposed to do, but it doesn't. Don't ask me why.

I don't really care either way, since you solved my problem.

Thanks for the help ... Chris

[Curtis_Waguespack]

Hi jtylerb,

---

jtylerbc wrote: I can't really come up with a situation where I wouldn't want the iProperty updating when I add a revision to the table.

---

This would be appropriate for companies that control revisions on items and documents both. Meaning that Part Number 123-456 is at Rev 3 but Drawing Number 123-456 is at Rev 6. The item and document are revised when the physical part changes, but only the document is revised for general note changes and things that don't impact the physical part, etc.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[cadman777]

I have another question off topic, if you don't mind:

Is there a way to establish a part view in the part file that can be accessed it in the idw file?

Reason I need that is I can't figure out a way to create in the idw file a view that's perpendicular to the c.l. of this part that's  not orthogonal to the default axes/planes.

... Chris

[Curtis_Waguespack]

Hi cadman777,

You can create any custom view you need by using the Change View Orientation button in the Drawing View creation dialog box.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[jtylerbc]

---

@Curtis_Waguespack wrote:

This would be appropriate for companies that control revisions on items and documents both. Meaning that Part Number 123-456 is at Rev 3 but Drawing Number 123-456 is at Rev 6. The item and document are revised when the physical part changes, but only the document is revised for general note changes and things that don't impact the physical part, etc.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

---

Ah, yes, that makes sense.  I've just never worked anywhere that treated it that way.  The drawing revision and the part revision have always been considered the same at the companies I worked at, but I can see the logic behind it.  It would have prevented some disputes I've seen where we got stuck with a tooling charge to change the rev letter on a part because of a minor drawing correction.

[cadman777]

Curtis,

Thanks for replying.

In order to simplify this, let me attach the part file.

It's a concentric reducer that I need to make views of that start wth perpendicular to the center line.

How would you do it in an idw file?
In SolidWorks, you can create any view in the model file, and then reference that view in the drawing module.

Inventor doesn't seem to have any way to do that.

Any ideas?

There are 2 files. I'll post one now and one in another message with no body.

... Chirs

[Curtis_Waguespack]

Hi cadman777,

Here are a few steps to do this (there may be other selections to create the work features that will work as well):

• Add a work point by starting the Work Point tool and then right clicking and selecting Loop Select, and then click the top inside edge of the cone.
• Do the same thing to add a work point to the bottom inside edge of the cone.
• Add a Work Axis by selecting the two work points,
• Add a Work Plane by selecting either of the work points and then the work axis.
• Click the View Face tool (View tab > Navigate panel)  and choose the work plane in order to set your view to the work plane.
• Right-click on the View Cube and choose Set Current View As Front.
• If this isn't really the view you want as the Front, select that view on the View Cube and then right-click on the View Cube and choose Set Current View As Front again.
• Create your view in the drawing.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[cadman777]

Curtis,

Thanks for thaking the time.

That's exactly what I did.

If you check my "Wireframe", you can see I have a plane in there already, which I exported into the part file.

I used that plane to view normal to it.

Then I did the rest of what you said.

Only thing I'm afraid of is the model reverting back to as-made view and then messing up the drg view.

I wanted a more permanent solution to this 'challenge'.

... Chris

[Curtis_Waguespack]

Hi cadman777,

I don't think you have to worry about the drawing view reverting back to anything. The drawing view is only using the "Front" view for creation, and doesn't rely on it afterwards. You can test that by using the Reset Front option if that helps.

Also, Inventor 2012  introduced View Representations for Part files that allow you to create and lock camera views to be used in the drawing as well.

http://inventor-tales.blogspot.com/2011/04/view-representationns-in-part-files-new.html

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[cadman777]

that's good to know

yeah, 2012 has a lotta new stuff, only i would need to buy a new machine to run it if i wanted to get any production out of it.

thanks ... Chris