Link Character Size to Dwg View Scale?

[LynnB1]

Hi all,

I am trying to use a Note on a print to represent etching on the part. Because the character height matters in relation to the size of the part, and the view scale is not 1:1, I need to update the Character Size in the style of the note. Now that in itself is very simple to do, I just enter .075*4 for the Character Size if I want .075 size text on a view that is scaled at 4:1.

Is there a way to somehow associate the view scale to the character size? If at some point down the road someone (or yes, even myself) changes the view scale and forgets to change the character size of the note, then the etching is no longer accurately represented on the print. I used to work around this by simply modeling the text into the master file, but I've recently been told that the preferred method going forward is to use Notes in the dwg file.

Is this possible, or should I have a little more faith in whoever updates these prints down the road?

NX8.5, TC10

 

[Kenja824]

It has to be done with a Note in Drafting? The only thing I can find that allows the text to scale with the view is if I add the text in Modeling thorough INSERT / CURVE / TEXT.

Someone else may know of a way, but this is the only way I can figure.

 

[LynnB1]

Kenja,

Adding the text in modeling the way you described is how I used to add the etch text. Always worked well for me in the past. There are reasons beyond my control that we will be moving away from that practice (unfortunately), so I'm just curious if there is a way to make it slightly more fool-proof when adding it on the drafting side.

 

[cowski]

I'm not well versed in the usage of PMI, but perhaps a PMI note would do the trick?

Here is an alternative that doesn't use PMI:
In the drafting application, turn off the sheet display; it will appear that you are now in modeling, but you are still in drafting. Create a note on the model, orient the WCS to the desired position before creating the note (the note will be created on the X-Y plane of the WCS). The note created will be view dependent in your current view; use the view dependent edit command to convert the dependency from view to model. Turn the sheet display on again and place a view on your drawing sheet (make sure that the view comes from your drawing file and not the model); the note will show in the view and will follow the scale factor of the view. While in the drafting application, you can expand the view to edit the note (note text or location) or delete it. The downside is that it is not an intuitive process and it may confuse your coworkers (or your future self) as to how it was created.

www.nxjournaling.com