MCX2 MR2 lathe will not output R's for arcs

[kcham]

This day as made me want to go back to programming by hand. I have been using MCX2 (initial release) since it came out. I am a lathe programmer, so I am using the lathe product. My employer recently bought me a new computer, and MCX2 MR2 was loaded into it for me. I have been using MR2 for about a week with only one minor problem, but today a major problem showed up out of nowhere. Suddenly, I started getting I/K output on my arc moves instead of R's. So I edited the control definition to "Radius" (I don't know how it got changed from this in the first place), but the output continued to be I/K. I played around with absolute the other arc settings to see if changes occurred in the output, and some did, but I never got R's. I went back to a file that I used last week (the output was OK) and it still outputs R's. However, in my investigations since, I have discovered that any new file, regardless of machine definition or postprocessor WILL NOT output R's even if I change the control definition settings. Any ideas? PLEASE HELP. Thanks.

[gcode]

Make sure you have read/write access to the X2

install folder

[kcham]

Some of it was read-only. I changed this and opened the control definition and saved it, but it made no change to the posted output.

[Thee Dragracer1951]

I'm thinking the pointer to your post is not right. Or as has been mentioned, your machine def and or control def are corupt

Have a look

There is a setting in the post as well as the control def that controls I&K's or R's

[Greg Williams]

Def works I have changed R to L. Perhaps you are using a different post with the same name?

 

 

(TOOL - 1 OFFSET - 101)

(PDJNR 2525M 15 - R08 INSERT - DNMG 15 06 12)

NAT2(FINISH FACE)

G97 G95 S=295 M41 M602 BA=45. M8 TL=001101

M4

MT=02001

G18

G0 Z5.

Y-20.

X420.

Z1.414

X383.341

G1 X380.513 Z0. F.25

X270.214

Z2.

(FINISH OD)

G0 X420.

Z5.

Z2.121

X362.87

G1 X367.113 Z0.

G18 G3 X371.513 Z-2.2 L2.2

G1 Z-77.988

X370.913 Z-93.693

Z-188.54

G2 X377.532 Z-196.469 L11.3

G1 X390.782 Z-203.094

G3 X395. Z-208.185 L7.2

G1 Z-243.766

X397.828 Z-242.351

G0 X500.

Z-230.

M05 M9

G0 X1500.

Y0.

G20 HP=4

TL=001000

[Colin Gilchrist]

Is your control definition pointing to the correct post? Are you editing your Control Definition through the Machine Definition Manager?

 

If you make your changes in the CD using the "Control Definition Manager", that change is made to the library copy of the Control Definition, but is not automatically transfered to the "MCX MD/CD copy". You must go into the Machine Group Properties - Files page, and use the "replace" button to reload the Machine Definition and Control Definition files from the Library copies.

 

If that doesn't work, feel free to email me and I'll help you sort it out.

 

Thanks,

[Redfire427]

kcham,

I will ask a dumb question here. Why would you not want i and k output instead of r output? Depending on how many degrees the arc is, you may end up with the wrong arc as there are two possible options unless you have arc break at 90 turned on.

Just a question.

[kcham]

Prosin Molds,

I use R's because that is what all of the machinists here are used to seeing, and it makes it easier to read the program at a glance. I always break my arcs @ 90degrees as a habit from my days of programming with a calculator.

Colin / Greg,

I have checked all of the paths and they are correct. I am using the machine definition to alter the control def.

Dragracer1951

I found a post in my system (recent MPLFAN) that would output the R like it is supposed to. The problem post is an old V9 post that has been altered and updated several times. I compared the arc settings in this with my problem post, and they are the same. However, I had a look at the 'parc' postblock, and discovered that they were very different. I copied and pasted this block from the good post to the problem, and now the problem post seems to be outputting as expected!!!

Thanks for all of the suggestions!

[crazy^millman]

I would strongly recommend moving to a X post as soon as possible. Legacy posts are going to cause you more problems down the road. They do not play nice with the machine def and the more Mastercam supports machine definitions and you keep these updated posts the more problems people like yourself are going to run into.

 

HTH

 

[ 05-13-2008, 09:08 AM: Message edited by: Crazy^Millman ]

[kcham]

Crazy,

Yes, I've seen what you mean several times now. I am in the process of altering a version of the new MPLFAN to my liking, but I am learning as I go and I still have parts to program in the meantime. So, for the time being, I am forced to fool with the same old stuff for a while. Thank you for the recommendation.