G41 offset & Mach2

[InventIt]

I am trying to get Mach2 to offset my cut to accommodate the dia of my cutter. I added a G41 to my G-Code file and drew the letter "T" in the picture. As you can see it traced around the outside edge of the inner T (drawn without offset). Everything looked good except for the three places it crashed into the inner T. I circled and marked them 1, 2, & 3 in the picture.

Anyone know why it did this?

[HuFlungDung]

That is a typical problem with some controllers trying to perform tool radius comp.

You are likely aware that you will never get those square corners with your tool anyway, so my advice is this: always radius every sharp corner. Even if it is just a tiny radius it may help. If you use your actual tool radius, it wouldn't hurt either, and the results would be identical.

This is theoretical. I do not have your controller to say one way or the other

[ger21]

I'm not sure if Mach1/2 works like this (read the manual), but I think you need to add a lead in move for G41/G42, which wouldn't work for what you're trying to do. I'd need to see your code to see where you put the G41, but typically where your first G1 is after G0, the tool is not offset. It offsets from the first point to the second point. For instance, with a 1/2" D tool:

G1 X1 Y1 ( The center of the tool is at X1 Y1)
G41
G1 X2 Y1 ( The center of the tool is now at X2 Y 0.75)

Hope that makes sense (and I did it correctly)

Gerry

[InventIt]

ger21, I understand exactly what your saying. I made my lead move between the start point (marked "end" in pic), and circle #1. It did offset the entire circumference of the letter. It just did not like the corners for some reason. Maybe I need a radius in every inside corner?

[InventIt]

Here is the GCode file. If anyone wants to take a look.

[ger21]

I just read through the manual, and it wasn't terribly clear (It's more confusing than it needs to be imo).

I would do what HU says and radius each inside corner the radius of the tool (I'd personally go a very small amount bigger to be safe). I was in a hurry earlier and didn't look close enough at the picture you posted. The machine I use at work doesn't have any problems with 90° inside corners, but apparently Mach2 does. You might want to ask this question on the Mach2 newsgroup (yahoo) as well.
Where did use to create the .dxf? you have some extra lines of code you don't need in there, from a sloppy .dxf. For example,

N34 X0.6396 Y0.8320
N35 X0.6279 Y0.8320
N36 X0.6162 Y0.8320
N37 X0.5498 Y0.8320

The middle 2 lines can be removed and you'll get the same results.

You might want to look at Outline Art from here:
http://www.freefirestudio.com/

I've had pretty good results from the demo.

Gerry

[InventIt]

I used DeskEngrave for the conversion.

Thanks ger21 and Hu, I'll try adding a radius and checkout the software link.

[bholterman]

When you offset an inside cut, the geometry gets crazey. You may end up with overlapping lines that you do not "see". Try offsetting line segments one at a time in the inside cut areas and you can see the problem develop. I just offset up to a trouble area like that and then join the offsets that are good enough for final geometry. Remember you are looking thru a microscope and the finished part will look different. Doing letters is difficult as they can be complex and perhaps a re-size would be easier...I reset the line width on the offsets to see a realistic preview of what the tool would do.