Since our shop will only work with inch dimensions, we have to dual dimension (have alternate units on) when we detail jobs. then for the final documents for the customer we have to turn off the alternate dimensions in all dimension styles. we have quite a few. I was wondering if there was an easier way to turn them off and on for all the dim. styles other than to edit all the dim. styles individually and turn them off and one?
thanks
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Will your customer not accept dual dimensioned drawings? seems a bit silly if they don't IMO..
Hi slphantom,
I might not be understanding, but I think I would have a dim style that shows the alternate dims, and one that does not. Then you would be able to Hold the Shift key and Right Click anywhere on the blank drawing sheet and choose Select All Inventor Dimensions, and then go to the Annotate tab and use the Styles pulldown to change them all to the other dim style.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
it is a pain in the butt for us for sure. no most will not accept. they all have very strict standards. which is fine, it is our shop that will not move to the metric system. sore spot with me for sure. we don't have one customer (automotive companies) that uses inch dimensioning.
Curtis, the problem with that is we are constantly changing the tolerances in dimensions being a gage company, so when you add a tolerance to a dimension if you change the style of that dimension the tolerance goes away.
@slphantom wrote:
Curtis, the problem with that is we are constantly changing the tolerances in dimensions being a gage company, so when you add a tolerance to a dimension if you change the style of that dimension the tolerance goes away.
Hi slphantom,
Dang, that does make it a challenge. Are you open to an iLogic solution?
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
sure if it would keep all the dimension tolerances and added text and just remove/add the alternate dim's.. I have just started teaching myself ilogic so I am very bad at it.
Hi slphantom,
Here is a quick rule that runs through all of the dims on the sheet and then toggles the the atlernate unit option for the dim style. Post back if you need to it look at multiple sheets, or something else.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
'Alternate Dim Toggle ' Set a reference to the select set of the active document. Dim oDoc As DrawingDocument oDoc = ThisApplication.ActiveDocument ' Find all selected occurrences and add them to an ObjectCollection. Dim oDrawingDims As DrawingDimension 'Loop through all dimensions For Each oDrawingDims In oDoc.ActiveSheet.DrawingDimensions ' Set a reference to the dimension style of each dimension. Dim oDimStyle As DimensionStyle oDimStyle = oDrawingDims.Style ' Modify the atlernate unit property of the dimension style. If oDimStyle.AlternateUnitsDisplay = True Then oDimStyle.AlternateUnitsDisplay = False Else If oDimStyle.AlternateUnitsDisplay = False Then oDimStyle.AlternateUnitsDisplay = True End if Next
Curtis, is there a way to use this type of Dual unit format? xx [xx] as shown in attached.
also the ordinate dimensions do not toggle after the first switch.
thank you very much. this is so cool.
Curtis, the ordinate dimension problem was on our end. Sorry, someone thought it was a good idea to use their own dimstyles. when i switche it back to our standard dimstyle it worked fine. I would still like to learn how to make it so the alternate dims are in the brackets like my post above.
Hi slphantom,
You had me worried there for a bit with the oridinate dims part.
Here's an update that will set the format.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
'Alternate Dim Toggle
'- - - - - - - - - - - - - - - - -
' kAdjacentFormat = 41985
' kAdjacentWithBracketsForPrimaryFormat = 41986
' kAdjacentWithBracketsForAlternateFormat = 41987
' kBelowFormat = 41988
' kBelowWithBracketsForPrimaryFormat = 41989
' kBelowWithBracketsForAlternateFormat = 41990
' kNoAlternateUnits = 41991
'- - - - - - - - - - - - - - - - -
' Set a reference to the active document.
Dim oDoc As DrawingDocument
oDoc = ThisApplication.ActiveDocument
Dim oDrawingDims As DrawingDimension
'Loop through all dimensions
For Each oDrawingDims In oDoc.ActiveSheet.DrawingDimensions
' Set a reference to the dimension style of each dimension.
Dim oDimStyle As DimensionStyle
oDimStyle = oDrawingDims.Style
' Modify the atlernate unit style of the dimension style.
If oDimStyle.AlternateUnitsDisplay = True Then
oDimStyle.AlternateStyleFormat = 41991
Else If oDimStyle.AlternateUnitsDisplay = False Then
oDimStyle.AlternateStyleFormat = 41987
End if
Next
thanks so much works great.
Hi Namoi1,
Much of this relies on the Inventor Application Programming Interface (API), you can find some links at this link, to learn more about iLogic and the API:
http://inventortrenches.blogspot.com/2013/10/ilogic-how-to-learn-inventors.html
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
There's a way to turn off alternate units: in the drop down menu in the styles editor.
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