Most Suitable Single Line Font for Engraving 1

[designer22]

Hi,
I am looking for a single line font suitable for engraving on CNC
I need to model this in NX8 and send to our machine shop for them to program on different CAM software
Can anyone please suggest one?
Thanks!

 

[Toost]

This has been discussed before here. If you search google i think you will find old threads on this. ( I remember John Baker had a long post on this.)
Anyway,
generally "Windows fonts" such as true type etc are never single line, and NX drafting fonts are mostly single line.
So one method is to create the text in Drafting application, but do not display a drawing. ( display the 3D model.)
Then you will need to place the WCS on the face of the solid where you desire the text to be created/engraved. ( +XC = reading direction)

Does this help or should i dive deeper ?


Regards,
Tomas

 

[BubbaK]

The traditional NX fonts are "stroked" fonts (as opposed to Windows TrueType fonts, which are "filled"). Among the NX collection, the most complete (and the most readable, in my opinion) are the Hershey ones. There is a serif version and a sans-serif version. The latter has fewer strokes, so would engrave faster, I suppose. Some of the other NX fonts have even fewer strokes, so they are faster/uglier.

 

[Toost]

If you prefer the European standard, ( and want a font similar to the Iso Standard for drawings) i would recommend "latin-extended".
It contains the European special characters.


Regards,
Tomas

 

[Rob_N]

I use the Modern font in NX for text that I plan on engraving in WorkNC

 

[Toost]

Here's an example of the NX Drafting font. ( including two NX engrave operations inside the same file. - No master model in this example)) NX7.5 file format.
I'm no expert on CAM, the machining parameters can be very bad. Creating these 2 operations is as simple as possible, maybe 4 minutes to setup.

Regards,
Tomas

 

[Rob_N]

Toost, Why not just use the Text command in modeling. Choose On Face, select the face. Placement, Curves of faces then select an edge to control the direction. Then the Modern Font, select my font ize and I generally check all 3, Associative,join curves and project curves in-case the face isn't planer.

The drafting font method I recall from many years ago.
I don't remember when I moved to this method, but its been awhile. I'm fairly sure it worked in 7.5.

 

[Toost]

I use drafting test because it's a "two click" operation to create the engraving NX operation in NX. ( it's quite a few more clicks than two but basically one only needs to pick the text and a floor plane. Generate.)
i agree that it's kind of old fashioned and non-associative, but, it's fast.

( Someday i guess that CAM development enhances the engraving operation such that True type text can be selected. - Mark ?)


Regards,
Tomas

 

[Rob_N]

One thing I did like about the Drafting note method is you could replicate a "text box".
With text curves in modeling you have to do each line as a separate feature.

I occasionally use some of the true type fonts like wingdings3 to engrave arrows and other symbols

 

[designer22]

Toost,
Thanks for posting the sample file

When we create a text in drafting, it's like note
It doesn't translate or export to stp file for our CAM department and CNC
Is there any solutions or different font to go in modeling
Thanks to everyone for the suggestions

 

[Toost]

I will have to withdraw my previous statements.
Drafting annotations doesn't translate to Step and i don't succeed in seeing that drafting note if i go master modeling.
The font Rob recommended, "Modern" should be the suggestion.

Sorry is i caused any confusion.

Regards,
Tomas

 

[Rob_N]

If you make the curves with the Text command in modeling they export out fine, it doesn't matter what font you use. Though Modern is a single line font. Some people my get upset if you send engraving curves out in Old English font
You have to make sure curves are checked though in the settings to be exported AND make sure Curves are set to be imported on the receiving system. by Default NX is set to import/export solids only for Step.

Before we moved to the NX direct translator for WorkNC, I stepped and/or Iges out models to be engraved daily