Possible bug?

I looked at your dxf file and you have some 5mm circles and I assume your trying to make holes from them with a 4.5mm tool. DXF2gcode generates an entrance move that is perpendicular to the arc and with so little difference between the hole size and the tool you can't make that move with cutter comp on. I deleted all but one 5mm hole to see what the comp move was after commenting out the G42 line you can see it. Free software is not clever enough to do such tight work and follow the constraints of an operating systems tool compensation system.

Deleting the 5mm holes I was able to come with a workable program in a few minutes with DXF2gcode by fiddling with the Start Radius setting.

John

2e0poz wrote:

Just to be clear when i said i do not add the compensation manually to the code. In the application you select left, right or centre. or outside, inside or middle on the other app.

Which options are you selecting? I would expect the correct sequence to be centre in the first app, then the correct side in the second. If you select an offset in both then you are likely to get a double offset, and curves too tight for the cutter.

To sort this out, how big is the first hole meant to be? And what does the G-code look like up-to and including the first G2 or G3 move?

2e0poz wrote:

Andy i am only using one or the other not both at the same time, the end result was the same which ever i used. I think John hit it on the nail with the fact the software is not clever enough to flag there is not enough room for a lead in with the size cutter i was asking it to use. For the small holes i told it cut right where it would be better to do a tool change and cut centre with a 5mm bit to match the holes.

Spiralling down is perfectly legitimate, but it probably makes sense not to try to do it with G42 active.

Incidentally, your hole pattern is a really good example of some code that could be efficiently hand-coded using the loop / sub conditional codes in the EMC2 version of G-Code.

Have a look at this section of the docs , if you are interested.
www.linuxcnc.org/docview/html//gcode_main.html#cha:O-Codes

Another useful tool is the Counterbore Simple G Code Generator.

wiki.linuxcnc.org/cgi-bin/emcinfo.pl?Sim...Counterbore_Software

John