Text engraving and single line fonts

[Davavanstone]

Hi, I'm using NX2212 and am having some trouble engraving text. I want to model the text for another machinist to manufacture. I don't want to simply extrude cut a font into the part, this is not machinable, corners cannot be machined, and it means a lot of toolpaths to cut the extruded face.

My font would need to be engraved with a 1mm ball end mill.

My current workflow, and this works for sketches, but no fonts, is to extract the surface, then offset the surface by .4 then draw a sketch on a plane at distance then project the curves to the offset surface. I would place a sphere at 1mm diameter at the corner of a curve or wherever required, then use swept volume with the sphere. This yields an "engrave" EXACTLY as it would be done when milled. If engraving on a flat surface, I skip the offset surface part and just use a sketch on a plane at .4mm away.


Now, the issue is fonts... I have scoured the internet for months for a TRUE single line/stroke font so I can engrave text in this way, I've found quite a few but they always fail with swept volume. The tool has very little verbosity, so I've no idea why it fails.

A work around is to put a sketch on the same plane, and "trace" the text into true geometric shapes rather than faceted curves. This works but it's very time consuming.

Do true single line TTF fonts that aren't faceted actually exist?

Is there something I'm missing on how to do this more efficiently?

 

[Toost]

Have you looked at the old "Unigraphics fonts" ?
True type was implemented in, i think, NX8.5, before that all fonts was single line.
These fonts still are included in the install but in later versions of NX you must enable these to appear in the session. Else you only see True type fonts in the dialogs.
Customer defaults- something ... ( im not on a computer where NX is installed at the moment.)
NX also has e very straightforward engraving option which uses these fonts.

Regards,
Tomas



The more you know about a subject, the more you know how little you know about that subject.

 

[Toost]

Here's the option :
( NX1980/2000)

Select the Standard and NX fonts, save the customer defaults , restart NX and you should see the old style fonts.
/ Tomas

The more you know about a subject, the more you know how little you know about that subject.

 

[Rob_N]

I use the "modern" font for text that's going to be engraved

 

[multicaduser]

Rob N, that's the font we user for "on curve" engraving even on doubly curved surfaces, but because it's a series of straight lines it's difficult to use if you want to simulate a ball cutter in 3d. I feel the pain of the process but there it is, and it's still better than other cad systems.

NX 2212 Windows 10

 

[Rob_N]

Mainly I use it for scribing text with a drill-mill. using a ball is tricky. I used to have a calculator. but lately, I just s

ave a couple of sequences once I got the width I wanted

 

[Matt P]

A solid answer for this would be amazing. I've had the same issue for a long time now and using Modern OEM/DOS font is an ok stop-gap but it causes issues from the design to machining as it can't be represented in solid easily meaning text curves also need to be provided in a machine file to be programmed against instead of just a solid or sheet body file.

 

[Levy1989]

I made an excel doc to calculate width of lettering when using a ball to engrave. The formula im using is width of cut = 2*SQRT(r^2-(r-DOC)^2) where r is radius of tool and DOC is depth of cut.

It is frustrating because I want a visual on my part when reviewing it not just a drafting text that isnt attached to the body.

 

[Rob_N]

Levy1989, does it work for DOC to the width of cut on freeform type surfaces for 5axis engraving? the one I used to have I could use say a 3mm ball to cut my max-min trim tolerance on check fixtures.

if so, can you share it?

 

[Levy1989]

Hi Rob, I have not done 5 axis machining. I believe it would work as long as the tool axis is normal to the surface while engraving.

 

[Rob_N]

Thanks Levy, thats similar to what I had before. Though it was the Radius of the tool and what WOC I wanted and it gave the DOC to achieve it.

To make a visual on the model, you could use this formula to offset your surfaces and project your trim or letters to it. then create a solid of your "tool" and use swept volume? granted its a lot of work.

 

[Levy1989]

Yeah that would be a lot of work!
I typically just extrude a regular font text into my model, then when I am in CAM I will add the drafting note and engrave it not ideal but gets the job done (luckily im only engraving on planar surfaces)