Circle Mill

[tnevy]

What our operators want is X and Y output at each point, and then the sub call generated by Circle Mill. Right now only the changing axis is output.

using force output in the Additional Holes section in the post doesn't help when using Circle Mill. Can anybody help? Thanks Tnevy

[roland_1]

Hi, I checked and I have X Y output corectly on forcing. I am now learning how to edit posts so in that proces I can do it for free. if you want send it and I will try to set it in yours. or if you dont want post here your code example and what you want to change. that is not so appropriate way, but I can try to explain!

[Guest Tnevy]

After first hole location and sub call, which is correct, we would like to force output of next x and y for next hole. I'll get some actual code from work tomorrow. We use circle mill to chamfer holes and to mill grooves inside holes. Things are working correctly, I'm just trying to keep operators happy. They never are for long, before they want more. Thanks Tnevy

[roland_1]

yes send that will explain much more in detail

[tnevy]

The following is a sample of our code.

 

N31G17G40G49G80G94G90

N32/M8

N33G0G43H19G55X-21.9375Y-4.375Z3.

N34S1800M3

N35Z.5

N36Z-.543

N37G1Z-.563F15.

N38M98P1002

N39G0G90Z.5

N40X-19.6875

N41Z-.543

N42G1Z-.563

N43M98P1002

N44G0G90Z.5

N45X-17.4375

N46Z-.543

N47G1Z-.563

N48M98P1002

 

What we would like is the y value in lines N40 and N45 and so on.

[tnevy]

Roland thanks for any help.

Tim

[K2csq7]

Use the post debugger to see where those lines are coming from in your post. In those lines you will most likely see "pxout, pyout, pzout, ....." Change them to pfxout, pfyout.

That will tell the post to force out the positions of X & Y even if they are the same as they were on the previously output line.

 

BTW, Always backup your post before editing!

[roland_1]

and where is Circular Milling in your code? It is in sub programs? I understood that you need both points in Circular milling.

You can do what K2csq7 said. you can just put simbol * in front of x and y outputs in your post.

but remember that it can cause the same output all the time when you will use that post. for all other operations.

if you want, you can send me all your files: post, MC part, machine definition, and I can try to put some additional code that will post this output of x and y onli in special cases that you want.

[tnevy]

I would like to use post debugger. I figured some how or somewhere I would be changing pxout and pyout to pfxout and pfyout. But I don't know where or how to use post debugger. Roland the circle milling is in the Sub.

 

O1002

N1G91

N2G41D19X.523

N3G3I-.523J0.

N4G1G40X-.523

N5M99

[K2csq7]

Post #9 gives the details on how to enable & use the post debugger.

 

My link

 

[roland_1]

in MC "documentation folder" that installs with MC software on your computer you have PDF lile with name Debugger Reference Guide.

thre are explanations. but you will need to spend pretty much of time to get all of that if you are new.

problem is that anybody cannot suggest to you exact sollution because for that one need a lot of information. and possible experiments. and also exact thing that you want. do you want that output all the time in every operation ect. and nobody knows exactly how your post is configured.

you know thats all are parameters.

[Guest Tnevy]

I tried the debugger today, I should have written down the exact line that needs to be changed, but I think it was xoutput and youtput. I added * symbol to make it like force output. Wow! WAY TOO MUCH code. I'll probably just drop the project, because I would have to find a way to and change the output ONLY for circle mill points. Since everything else is OK.

 

Tim

[roland_1]

yes that is the case. if you change it, all code will change.

I can tell you right now that you will have long time to go till you fing how to change just for circle mill sub program call. if you want start to look how to deal with parameters.

but if you want send me all your files end I can take a look for weekend.

[K2csq7]

if opcode$ = circle mill, (*xout, *yout)

else, xout, yout.

 

Sorry I don't have a lot of time today to look up the place to put it or the opcode for circle mill, but if you have the time & have backed up your post at the very least it will be a learning experience!

-Start

-all programs

-mcam

-documentation

-nci & param ref guide

 

That pdf will have the opcode & it looks like you already know where to put it.