Dimension text position as dimension changes.

[Anonymous]

Situation:

13 Parts, 1 Assembly, 1 Drawing (14 sheets)

The Drawing File contains the Assembly on page #1 and one part per page after that.  

The project is meant to be used as a configurator (via ilogic design copy and then updating parameters as needed), while the resulting drawing becomes our production drawings.

My problem is that the placed dimension in the drawings are updating uppredictably as the assembly changes size, particularly as the dimesnions shrink.  See the picture for examples.  

What methods are available to solve this issue?  Is there a way to create the dimensions in a way that they stay centered between the extension lines?  Is there a command, tool, or ilogic code that could auto-update these for me?

Thoughts, suggestions, and alternate stratagey sugestions welcome. 

[Mark.Lancaster]

DImensional cleanup is always going to exist.  You are changing the size of your parts and Inventor is not going to automatically recenter and fix all the dimensions and views for you.   I suppose a program coould be written to recenter all your dimensions but nothing out of the box is going to do that for you.

[Curtis_Waguespack · Accepted solution]

Hi Matt.Carter,

Have a look at:

Tools tab > Options panel  > Document Settings button. In the dialog box, click the Drawing tab.

Dimension Updates

Dimension Text Alignment Controls text position for angular and linear dimensions when geometry is updated.

• View Position maintains text position on the sheet.
• View Position and Maintain Centered Retains centered dimension placement, while all other dimensions maintain their positions on the sheet.
• Percentage of Dimension Line Attempts to maintain all dimension text positions relative to the dimension line.

There is also a related setting for controling how the dimension text is placed intially:

Tools tab > Options panel  > Application Options button. In the dialog box, click the Drawing tab.

Center dimension text on creation

Sets the default position of the dimension text. When creating a linear or angular dimension:

• Select the check box to center the dimension text.
• Clear the check box to have dimension text follow the mouse.

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

[Anonymous]

Then a rule or program is going to be the direction I need to go.   I am not opposed to this solution, I just need to be pointed in the right direction on the how.  

The concern in this case is that we plan to produce hundreds of drawings at a time by setting up the parameters in excel and pulling them in as part of the save-as process.  My initial test run is of 150 drawing sets. A manual check and correction of each individual page would be prohibitively time consuming

[Anonymous]

Thanks Curtis!

This will do what I needed. Now to just go make sure everything is centered

Thanks Again!

[Mark.Lancaster]

@Curtis_Waguespack  Thanks for reminding me about that option..   I forgot all about it since that option wouldn't work at my last place using our iLogic code.  Too many dimensions in a given view so it was impossible to have all the dimensions centered...   We always tried to jam 20lbs worth of information in a 5lb drawing....    

[Curtis_Waguespack]

@Mark.Lancaster,

I'm happy to help. I've not actually experimented with getting that to work with iLogic controled updates yet, but have just recently made a mental note to look into to it, as part of on going projects. 

I suspect I'm going to run into the same 20lbs to 5lbs issue as well. So thanks for the heads up.