[80083r]

I'm not sure where to even begin. I've been banging my head off of this problem for a week now.

I am making a jig out of 60" x 120" MDF (don't laugh - our tolerances are +/- 1/16 of an inch, give or take), just simple pockets used to drill holes in crimped window frames for mounting holes. The pockets are simple, done, woohoo.

The problem is - I need to scribe some text on each pocket, to show orientation of the frame, as well as the fixture#, part#, etc. It's a fair amount of text on EACH pocket.

I am using inventor to generate the model, and EdgeCAM 2009 (I'm hoping to have 2010 R1 installed sometime this year... a whole other story).

I can emboss the text, but I'm using a 3/8" router bit to cut the pockets and would like to cut the text with that also. Making the text large enough to fit a 3/8" router into makes it too big to fit into the space I have (don't even get me started on not being able to cut a 3/8" slot with a 3/8" tool due to links/leads).

I cannot leave the text in a sketch, Edgecam doesn't import sketch geometry. I can't export the sketch as .dwg or .dxf, the text doesn't get exported. I can't use text mill on embossed text.

I have called Inventor tech support and Edgecam tech support, and both are flummoxed.

I don't really care what the solution is, as long as I don't have to profile the whole embossed text and cut all the edges, or draw centrelines for everything.

Anyone have any ideas? How do you cut text in EdgeCAM?

[Teps71]

Can you "draw" the text in EdgeCAM (Geometery, Text) in design mode and use the Text milling cycle in manufacture mode?

I've used the simplex font which is a single point vector font and machined it with a 90 degree mill/drill with great success.

[80083r]

I can, but I was hoping to avoid that - as inventor is much easier to create text in, and it can be dimensioned and placed with precision. So far everyone is telling me it cannot be done - which just rubs me the wrong way.

I KNOW I can bring in text from .dxf and it works fine. I also know that I CANNOT import .dxf files. I can *OPEN* them, as long as I open them first, otherwise I have to open them in a new file, save as edgecam format, then go BACK to the original file and import the edgecam formatted 2d geometry.

[inflateable]

I had similar problem, and I gave up with edgecam. You can do it, but the files are huge and it's a massive headache to change text each time, with lots of back and forwarding of files, and it was just too slow and clunky. I did it the way Teps71 suggest above. Make sure you do use simplex font, it makes the file sizes a bit more manageable.
I was engraving on a flange diameter though, which added another level of problem.

I endedup getting a program called 'millwrite' which is absoleutly fantastic for engraving and text work, and not too expensive. Couple it with a spring-loaded engraving tool and it's brilliant, I can generate code for the text as fast as i can type it into the program, hit 'send' and the machine is running. I'm even putting the company logo on our parts with it.

You can get a demo here: http://www.hugequestions.com/MillWri...e-v6-demo.html


Just had a peek at millwrite's website, and they've now got an even simpler etching program, which sounds ideal for you. http://www.hugequestions.com/MillWri...ite_index.html and is cheaper.

[jsanders]

I can, but I was hoping to avoid that - as inventor is much easier to create text in, and it can be dimensioned and placed with precision. So far everyone is telling me it cannot be done - which just rubs me the wrong way.

I KNOW I can bring in text from .dxf and it works fine. I also know that I CANNOT import .dxf files. I can *OPEN* them, as long as I open them first, otherwise I have to open them in a new file, save as edgecam format, then go BACK to the original file and import the edgecam formatted 2d geometry.

Yes, Inventor is a CAD tool and is the best place to do part design. The resulting 'lettering' is easily handled by machining the entire solid rather than trying to get individual features. It's a really easy process. Here's what you do:

1. Create the Inventor solid with embossed text.
2. Use the Roughing and Profiling cycles to machine the solid, using a containment to keep the tool in the pocket if that is what you want.

Hope that helps!
Joe

[inflateable]

[QUOTE=jsanders;746028][*]Create the Inventor solid with embossed text.[*]Use the Roughing and Profiling cycles to machine the solid, using a containment to keep the tool in the pocket if that is what you want.[/LIST]



That snag with that is it only works if you want to make BIG characters. If you just want to engrave some text with a line thickness of (say) 0.2mm, that won't work.

[jsanders]

That snag with that is it only works if you want to make BIG characters. If you just want to engrave some text with a line thickness of (say) 0.2mm, that won't work.

No problem. See that attached files (my HAAS post isn't included ). Inventor 2010 + Edgecam 2010 R1. Design has 4 pockets, and each one has text that is 0.120" wide x 0.05mm height. The text is 0.0152" letter width and 0.0147 letter spacing. Edgecam builds toolpath with a 0.01" end mill, easily profiling the embossed letters.

ANSI Text that is 0.2mm line thickness (0.0078 inches) has a 0.001 spacing between characters. That is certainly a tooling challenge.

[80083r]

I appreciate the "machine solid" approach - but even those letters are a challenge. Remember, I want to use a 3/8" endmill and make the letters the width of the tool, my actual part is 5' x 10' and I need to be able to see the lettering from 20' away.

(I couldn't look at your file, my IT dept. is dragging their feet installing 2010 - I'm still using 2009 R2)

[rider23]

I am having a similar problem with edgecam and part modeler. Part modeler works great when it comes to sizing , placing and editing the text, converts great to edgecam as a dxf, but I cant find a text where the letters are a single line, all the fonts that I've looked at are doubled lined. is it possible to add a font style to the programs ?
The best that I am able to do is have a friend make the text on his Bob Cad program that has a single line font and then import it into my file.

[80083r]

I found a way to work around this issue, but it's not pretty.

First, I made a 1:1 drawing (temporary, I didn't save it) and exported the 2d as a .dxf. Then I opened the dxf in Edgecam, then I imported the solid.

The text wasn't quite the right size, but it was "text". From there I edited the text size/type in Edgecam and used text mill to cut the text.

[80083r]

I know this is resurrecting a very old thread - but it keeps coming up in a search and I hate threads with no answer - so I thought I'd update with my eventual solution to the issue.

now what I do is engrave the text in the model and I don't use it for anything except reference. I use the "text" under the "geometry" menu in Edgecam to make text of the approximate size and use dynamic move to place the text approximately where it's supposed to go. Its inelegant and kludgy, but it gets the job doen.