Delta 20 post processor/ code issues

[Kevin77]

Hi guys,

I have a Tree J325 mill with Delta 20 control. I'm trying to get a working post together for Dolphin. Where I seem to be running into problems is with cutter compensation, i.e. G40, G41, G42. The control doesn't like the code, and gives Error 133, "Format Fault." Here's a sample of some code:

(TEST2)
N5T1E1S1000M03$
N15G00G40X-0.6426Y1.159F80.0$
N25Z0.02$
N35G01Z-0.3$
N45G41X-0.18Y1.2269D1$
N55G02X0.18I0.0J0.0$
N65G01G40X0.6426Y1.159$
N75G00Z0.5$
N85X-0.6426Y1.159$
N95Z0.02$
N105G01Z-0.32$
N115G41X-0.18Y1.2269$
N125G02X0.18I0.0J0.0$
N135G01G40X0.6426Y1.159$
N145G00Z0.5$
N155M30$
END


It faults at line 45. Any ideas?
Much appreciated,

Kevin

[Southbend Sam]

My disclaimer, I have a lot of trouble with cutter comp too. That said, the Dynapath manual I have (under the G41 section) says that the diameter offset will only occurr in the selected plane (ie G17). The examples of cutter comp programs in the appendix set the plane with G17. Perhaps if you add a G17 line, that would help. I also use Dolphin as my cad/cam system and am currently using the post for Dynapath on their website and it does cause me to do a lot of manual editing of the code it outputs to get it to work. So if you get a working post I would be interested in seeing it.

[Kevin77]

Thanks, I will try that in the morning. What control version do you have? Have you noticed any issue with it only recognizing one Gcode per line? I.E. if G01 and G40 are on the same line, when I transfer the program to the control, only G01 shows up. Also, do you need to add "$" to the end of each line as an EOB character? The post processor I'm using doesn't include it, but I have to add it manually to get the control to accept the file transfer.

Thanks again,
Kevin

[Southbend Sam]

I am not exactly sure which version of Dynapath 20 I have. The mill its on is a mid 90's Hurco MHP. For EIA/ISO programming, the manual states only one G code per line. This is one of the problems I have had with Dolphin's post which produces multiple G coes per line. I have always edited the post output back to one G code per line. As far as the $ is concerned, when I download the code, either via RS 232 or by hand and am using EIA/ISO, it doesn't matter. I have noticed when viewing the code when the control is actually running a program that the control has automatically added the $ at the end of each line. If you are generating code in the conversational format, it is my understanding you need the $.

[Kevin77]

Well, adding the G17 did nothing. However, in Dolphin, you can disable "part surface programming," such that Dolphin generates code with the cutter comp built right in. Thus, there are no G40, 41, 42. This works fine. The only drawback is that you can't fine-tune a part by making small changes to the cutter diameter at the control. You have to change it in the cam and repost. Less of a hassle than hand editing lots of code though.

Kevin

[Southbend Sam]

That sounds good. How does one disable part surface programming? Thanks.

[T0DD]

Greetings Kevin-
The Delta 20, while heavly based on Fanuc, does not have the option of using whatever radial & lenght offset you want. Thus you shouldn't (can't) output "D#". Nor do you use G43 H# (which you weren't). Both of these are tied to the tool # and as such won't be specified in the G-Code. Also, due to the event method of the editor, only one G code per line is allowed. A G01 would be on the Z move, then G41 on the comp move. Please advise if this doesn't make sense. I don't know what Dolphin is, but I could look at altering the post if needed, unless you want to get UGNX, then I could quickly write a post. Also, I didn't see a feedrate output.

Take care,
Todd

[T0DD]

Ok, I see the feedrate output, strange place to put it, but if works, it works! Also at the end of path, you have two G-codes on one line. Pain in the butt compared to Fanuc controls, but who has the money to swap it out? I love my J425, not my delta 20!
Todd

[Fighter]

What works for me is adding a G1 line to the same position before the G41,42. The G1 needs to be at least the cutter diameter in length.

It needs to know what direction it is going in in order to comp correctly.

Try this:
N5T1E1S1000M03$
N15G00G40X-0.6426Y1.159F80.0$
N25Z0.02$
N35G01Z-0.3$
N40G1X-0.18Y1.2296
N45G41X-0.18Y1.2269

Dunno what the "D1" is for as I've never seen or used that.