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Shouldn't Inventor know that this is a cylinder and should therefore have a diameter symbol? Let's have it pop in there on its own without me having to do an edit text operation on it and manually add it.
I have seen similar discussions about this, but I have not seen this idea as a solution.
I work at a company that makes rotating equipment, so a majority of our drawings have many diameter symbols all over them.
I know that the diameter symbol automatically comes in when you actually pick the line representing the diameter, but that isn't always possible.
I know how to place them manually, but I would like to see an easier way to place them in front of the dimensions. Right now I go to the text tab of the dimension dialog box and have to arrow to the beginning of the dimension, and then select the dropdown and select the diameter symbol.
I would like to be able to pick the 2 lines that represent the diameter, place the dimension, and have a pickbox for the diameter symbol.on the front screen of the dialog box that pops up, and have it place the diameter symbol at the front of the dimension. A much simpler one click to replace the 5 or 6 that I have to do now.
AutoCAD Mechanical does this now, it would be nice to have Inventor have the option.
I have button with macro for write or erase diameter. Only select dimensuion and push macro button.
Public Sub PrumerPredKotu() If Not ThisApplication.ActiveDocument.DocumentType = kDrawingDocumentObject Then MsgBox "Funkci lze použít jen ve výkrese." Exit Sub End If Dim oDrgDoc As DrawingDocument Set oDrgDoc = ThisApplication.ActiveDocument Dim AList As Sheet Set AList = oDrgDoc.ActiveSheet If oDrgDoc.SelectSet.Count < 1 Then MsgBox "Musí být vybána kóta" Exit Sub End If Dim i As Long Dim counter As Long counter = 1 Dim VybranaKota As DrawingDimension For Each VybranaKota In oDrgDoc.SelectSet If VybranaKota.Tolerance.ToleranceType = kReferenceTolerance Then VybranaKota.Tolerance.SetToDefault VybranaKota.Text.FormattedText = "(" & ChrW(216) & VybranaKota.Text.FormattedText & ")" Else If Left(VybranaKota.Text.Text, 1) = ChrW(216) Then VybranaKota.Text.FormattedText = Mid(VybranaKota.Text.FormattedText, 2, Len(VybranaKota.Text.FormattedText) - 1) ElseIf Left(VybranaKota.Text.Text, 1) = "(" And Mid(VybranaKota.Text.Text, 2, 1) = ChrW(216) Then VybranaKota.Text.FormattedText = "(" & Mid(VybranaKota.Text.FormattedText, 3, Len(VybranaKota.Text.FormattedText) - 3) & ")" ElseIf Left(VybranaKota.Text.Text, 1) = "(" Then VybranaKota.Text.FormattedText = "(" & ChrW(216) & Mid(VybranaKota.Text.FormattedText, 2, Len(VybranaKota.Text.FormattedText) - 2) & ")" Else VybranaKota.Text.FormattedText = ChrW(216) & VybranaKota.Text.FormattedText End If End If counter = counter + 1 Next End Sub
This is an awesome script. I did some transalting and made the English version. I have been looking for a tool to do this very thing. We are a bearing manufacturer and everything we draw is round. I'm always and forever adding the diameter symbol to the 50 plus sheets I work on everyday.
I assigned the macro to the hot key "DD" Made it way easier to use. It even works when selecting multiple dimensions at the same time. This is too sweet.
Thanks!
Oh and by the way here is the English translation.
Public Sub DiameterInsertTool()
If Not ThisApplication.ActiveDocument.DocumentType = kDrawingDocumentObject Then
MsgBox "This function can be used only in the plot."
Exit Sub
End If
Dim oDrgDoc As DrawingDocument
Set oDrgDoc = ThisApplication.ActiveDocument
Dim AList As Sheet
Set AList = oDrgDoc.ActiveSheet
If oDrgDoc.SelectSet.Count < 1 Then
MsgBox "You must select the dimension that you want to add the diameter symbol to so the macro knows where too put the Diameter symbol!"
Exit Sub
End If
Dim i As Long
Dim counter As Long
counter = 1
Dim SelectedDimension As DrawingDimension
For Each SelectedDimension In oDrgDoc.SelectSet
If SelectedDimension.Tolerance.ToleranceType = kReferenceTolerance Then
SelectedDimension.Tolerance.SetToDefault
SelectedDimension.Text.FormattedText = "(" & ChrW(216) & SelectedDimension.Text.FormattedText & ")"
Else
If Left(SelectedDimension.Text.Text, 1) = ChrW(216) Then
SelectedDimension.Text.FormattedText = Mid(SelectedDimension.Text.FormattedText, 2, Len(SelectedDimension.Text.FormattedText) - 1)
ElseIf Left(SelectedDimension.Text.Text, 1) = "(" And Mid(SelectedDimension.Text.Text, 2, 1) = ChrW(216) Then
SelectedDimension.Text.FormattedText = "(" & Mid(SelectedDimension.Text.FormattedText, 3, Len(SelectedDimension.Text.FormattedText) - 3) & ")"
ElseIf Left(SelectedDimension.Text.Text, 1) = "(" Then
SelectedDimension.Text.FormattedText = "(" & ChrW(216) & Mid(SelectedDimension.Text.FormattedText, 2, Len(SelectedDimension.Text.FormattedText) - 2) & ")"
Else
SelectedDimension.Text.FormattedText = ChrW(216) & SelectedDimension.Text.FormattedText
End If
End If
counter = counter + 1
Next
End Sub
And also, thank you sgwilliams for converting it to English. I was going to do it later when I had time.
Now I don't have to wait to use it.
I still think it would be nice to have a button built it to do this.
Anytime glad I could help. I actually have installed this on the three Inventor stations in our Engineering office....these guys are all smiles....It's like it's Christmas time or something..
I totally agree with the button statement. This should already be a feature in the software. We should not have to VB gods to get simple things accomplished. But it is what it is. Inventor is still the cats meow, I remember when we had too draw this stuff on paper vellum and then make copies with special blue print paper and stinky chemicals...ahhh the good old days...even my dry cleaned lungs miss those days...NOT!
I think you must have something wrong. I have tried all different types of tolerancing and all work just fine for me. I even tried selecting multiple dimensions with a different type of tlerancing for each one and it still worked ok for me.
How do you have the macro setup? Is it setup ion the DocumentProject or is it in the ApplicationProject on the VB editor interface?? This might cause it to work differently. I will try that senerio tomarrow I have to shut the plant down and go pick up my grandaughter.
I tried it in the DocumentProject and realized you can't add it to a hot key when it is in this project. So make sure that you follow these steps to add it to your system.
1.When adding this macro create a new module in the "ApplicationProject (Default.ivb)" then select the macro and paste the script into it.
2.Then select the Tools Tab>Customize, a Customize dialog window will appear select the Keyboard Tab>Catagories>Macros. 3.In the Keys Column select the empty field and enter your hot key that you want to use to run the macro and then hit apply.
why you don´t use the ability of different dimension styles?!
So if you place a dimension you are able to switch this style with one mouse click.
I´ve got different styles for example Diameter symbol as präfix or "x 45°" as suffix
Michael, I'm old school and do most things with a keyboard, the mouse is useful for somethings but I was designing things long before the mouse was used in creating CAD geometry. Back in the day when AutoCAD 11 or 12 came out, not sure it was early 90's if I remember right we did not have a mouse as an option at my company. Management finally allowed us to purchase a mouse on release 13. So this has kinda been the way I learned, without a mouse,and the keyboard for me seems to feel more natural and faster. When I can select multiple dimensions and then just hit a hot key rather than finding the annote tab then going to the dropdown for the Style. Everyone has their preferences. It's hard to teach old dogs new tricks. I have alway's been a keyboard jockey and I doubt that will change.
I already have some things that use the style editor for but it is native to that feature like for the angle it has the symbol our company uses and the tolerance required. All in all I think when a dimension is pulled from a diameter wether it is single point or two point pulled it should automatically show a diameter symbol, the software is not smart enough to do this yet. If I set the prefix with the diameter symbol on my default dimension style it would show on all dimensions even those that are not round. Hopefully Autodesk will fix this someday, if they don't there is always VB.
Im really baffled why this has so many up votes. Make dim styles with the preceding diamter in your template/library, select all the dims you want on the same style then select it. Does it all in one go.
There is even the match properties button now but the style is faster.
CadUser46, We are all creatures of habit. We all find ways that make using software easier for each individual person. Your way may be easier for you but is very annoying too me. I would rather not have to set up 30 different dim styles. Your solution is too select a dimension or dimensions and then use the drop down to add one of your 14 styles too. Or choose the style before you create each dimension. My solution is too select a dimension or dimensions and hit a hot key. There really is no difference other than yours uses a drop down and mine uses a hot key. I do not see a drastic difference other than personal preference. I do not like the clutter of all those styles and having to sift thru them to achieve the same goal, for me personally I would rather hit a hot key then have to deal with 30 different styles. It may be efficient for you but it would not be for me, it would slow me down. I do however use the copy properties feature very often when dealing with multiple dimensions that use the same tolerance and precision. This is a great feature. Most of our dimensions are 4 place decimals as we make precision bearings. Each dimension usually has a different tolerance than the next so the copy properties helps but the actual tolerance upper and lower have to be entered manually. It is tedious work for sure but necessary. If I did more fractional or 2 to 3 place decimal dimensioning I would consider looking at your solution. Your solution woulds not work for us because we would have to set up twice as many styles as you have and it would be more time consuming having to choose which one too use and then manually put in the correct tolerance.
Just my 2 cents worth.
Hope that helps you understand why. We have 3 other engineers in our office and two of them prefer my solution. The other does not use either he just does everything manually. Each too his own.
You may like to look into the 'retrieve model dimensions' feature. Set all your dims and tolerances when modelling the part and you can just include them in your drawing. This would pull in the diameter symbol automatically i think.
You may like to look into the 'retrieve model dimensions' feature. Set all your dims and tolerances when modelling the part and you can just include them in your drawing. This would pull in the diameter symbol automatically i think.
Yes we tried this feature back in Inventor version 7 and it was decided by management that we would not use this feature because it was glitchy back then (2006) I think. New management lets us free to engineer as we choose so long as it doesn't interfer with our production schedule. So this is something we may look back into too see if it has been fixed since Version 7. I will have to play with this feature to determine its viability. Thanks!
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