Detail View Diameter

[Talayoe]

Good Day all,

Been using inventor for a few years now and have always wondered this question; Is it possible to dimension a diameter from a detail view.

I have given an example below from what I was working on. The part it was taken from was Ø29.200 at the largest diameter of the o-ring groove. And putting this on a B-Size drawing obviously crowds the dimensions into blurry lines. So the question remains, can I diametrially (is that a word?) dimension the detail view somehow?

Thanks!

[Anonymous]

Hi Talayoe,

Yes you can do the "Good ol draftsman’s" foreshortened dimension. Its fully linked and updates with the model.

Its a bit of a faff so I don’t use it much now.

1. Name the dimension for reference

2. Create your views etc... start a sketch on the detail view, draw a line to represent a centre line, change the properties to "sketch Only"

so it won’t show in the final drawing. (edit - do this last, after you have dimensioned your drawing)

edit the dimension select "hide dimension value". Click the edit pencil,

select the groove dimension (the one we renamed for ease of finding)

change the required decimal places and insert the linked dimension valve.

3. Create a double arrow sketch symbol and place it over the dimension (size shape to suit your style).

4. Print 🐵

[SBix26]

Yes, this is possible.  In your detail view, go to the browser and include the axis that defines the center of your diametral features, typically one of the origin axes (if not you may have to create a work axis just for this purpose).  Dimension from this axis to your detail features, but before placing the dimension, right click and select Dimension Type > Linear Diameter.  If the included axis is visible on your drawing sheet, you can turn off its visibility when you're done dimensioning.

Sam B

Inventor Professional 2018.1.2
Vault Workgroup 2018.0
Windows 7 Enterprise 64-bit, SP1

[stephenrottloff7259 · Accepted solution]

Hi Randy, it is possible.  The trick is to be able to include the hole's central axis within the detail view.  You can create the diametrical dimension then hide the axis if needed.  After the axis is included within the detail view, select the dimension command, select the included axis first, then the hole diameter geometry, right click and select dimension type, then Linear diameter.

I attached a screen capture showing the model tree and pointing to the included x axis.

Hope this helps,

Stephen R.

[Talayoe]

Hello Fellows,

Mark, thank you for the time and detail you put into that. Appreciate it. It does seem very cumbersome and I wouldnt use it much either like that. But I appreciate the input.

Sam & Stephen, both of similar replies. I tried it and it works fantastic and is very easy this way! Appreciate the input! 🙂

Tks!

[rpeterson9DZ38]

Awesome, I did not even think to do this.  

Thanks