Inventor & EdgeCAM scribing text

[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]

Originally Posted by 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.

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]

Originally Posted by inflateable 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.