Is there at way to make inventor round measurements on 2D drawind up/down to nearest fives?

[mbpUYRD7]

My boss doesn't like numbers there doesn't end with Zero of Five, where the precision aren't needed.

My questoin is, is there at way to make inventor round measurements on 2D drawings up/down to nearest fives?
so that meausrements like 522 are changed to 520, and 438 are changed to 440?

I know, I just can overwrite med measurements manually, but that is very "dangerous", as the measurements then not will update, if the parts are edited.

An example:

[johan.degreef · Accepted solution]

No, but you can add your request to this idea.

https://forums.autodesk.com/t5/inventor-ideas/precicion-primary-unit/idi-p/12482819

a checkbox "0&5" should do.

[mbpUYRD7]

OK, thank you very much for your reply, even though is isn't what I hoped for 😉

I have done as you suggested, added my request and voted for the idea you linked to.

[Frederick_Law]

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@mbpUYRD7 wrote:

My questoin is, is there at way to make inventor round measurements on 2D drawings up/down to nearest fives?

I know, I just can overwrite med measurements manually, but that is very "dangerous", as the measurements then not will update, if the parts are edited.

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Been there, done that a few times.

Tell your boss to follow ISO, ANSI and ASME standard.

You're 1000% correct on not overriding dimension in drawing.

If dimension really doesn't matter just model them to that dimension.

[Alexander_Chernikov · Accepted solution]

Hi, You can try such iLogic Rule

(instead "RndTo = 5" you can use other number, forex, 10)

' *** Alexander Chernikov, KHADI, 2023-0404 ***
Sub Main() ' Round_Dim_Up to 5
  Dim oDoc As DrawingDocument = ThisApplication.ActiveDocument
  Dim oSheet As Sheet = oDoc.ActiveSheet
  Dim oDrDim As DrawingDimension = ThisApplication.CommandManager.Pick(kDrawingDimensionFilter, "Select Dimension")
  Dim RndTo As Integer = 5
  Dim dPrec As Double = RndTo / 10 ' in iLogic dimension in cm!
  oDrDim.Precision = 0
  oDrDim.OverrideModelValue = Int(oDrDim.ModelValue / dPrec + 1) * dPrec
  oDrDim.Text.FormattedText = "<DimensionValue/>" + "*"
End Sub

[CGBenner]

@mbpUYRD7 Did the information provided answer your question? If so, please use Accept Solution so that others may find this in the future. Thank you very much!

[mbpUYRD7]

We have inhouse production, so my boss do (with good reason) not care that much about those standards, only those there makes sense for our production, and those precise measurements doesn't really, they only serve to make the people in the production waste time cutting the pipes in precise measurements instead of nice round numbers.

I know I can write me out of that in the 2D with tolerances and stuff like that.. but it would still be really nice, if it were possible to make Inventor just put the numbers in 5' and 10's, so hopefully that option will be added at some point of time.

I do for most part make the models in 5´s and 10's, but sometimes that aren't possible in the 3D, because of pipes going in an angle, or being attatched to fittings and other bought parts there aren't in 5's and 10's, making it impossible to make it all constraints fit, if all the pipes are made in 5's and 10's, but we are working with pipes there in real life can be bend a little and thereby easily can be made fit where they shall fit, even it they are a few milimeters of.

[mbpUYRD7]

That suggestion looks interesting, but I do unfortunately not know anything about that kind of iLogic rules, like where to put that code or how to use it.

[Alexander_Chernikov · Accepted solution]

Hi,

1. near Model tab press "+" and select "iLogic"

2. In iLogic tab click RMB on Drawing and select "Add Rule"

3. Enter Rule name and insert given code into

then Save it and Close window

4. Than You can run it by RMB

More information about iLogic at

https://help.autodesk.com/view/INVNTOR/2025/ENU/?guid=GUID-AB9EE660-299E-408F-BBE1-AFE44C723F59

[mbpUYRD7]

Thank you very much for the explanation. I appreciate it 🙂