The never-ending saga of the Hurco that's "ready to make parts"

[JimDawson]

Re: Code issue, please help. This stopped being fun a few days ago.

This may help to get you started, copy the following text into notepad and save into the CamBam system folder as Hurco.cbpp (C:\Documents and Settings\All Users\Application Data\CamBam plus 0.9.8\post) or where ever yours is at This should be a good starting point.



<?xml version="1.0" encoding="utf-8"?>
<PostProcessor xmlns:xsi="http://www.w3.org/2001/XMLSchema-instance" xmlns:xsd="http://www.w3.org/2001/XMLSchema" Version="0.9.8.0">
<Notes>Hurco KM3P Post</Notes>
<PostFile>{$comment} Made using CamBam - http://www.cambam.co.uk {$endcomment}
{$header}
{$mops}
{$footer}
</PostFile>
<Header>{$comment} {$cbfile.name} {$date} {$endcomment}
{$tooltable}
{$cbfile.header}
%
{$units}
{$distancemode}
{$cuttercomp(off)}
{$toolchange(first)}
{$clearance}</Header>
<Footer>{$clearance}
{$spindle(off)}
{$endrewind}
{$cbfile.footer}
</Footer>
<ToolChange>{$clearance}
{$comment} T{$tool.index} : {$tool.diameter} {$endcomment}
T{$tool.index} M6</ToolChange>
<MOP>{$comment} {$mop.name} {$endcomment}
{$toolchange}
{$velocitymode} {$workplane}
{$mop.header}
{$spindle} {$s}
{$blocks}
{$mop.footer}
</MOP>
<CannedCycleStart />
<UnitsMM />
<UnitsInches />
<VelocityModeConstantVelocity />
<Rapid>{$g0} {$_x} {$_y} {$_z} {$_a} {$_b} {$_c} {$_f} </Rapid>
<FeedMove>{$g1} {$_x} {$_y} {$_z} {$_a} {$_b} {$_c} {$_f} </FeedMove>
<ArcCW>{$g2} {$_x} {$_y} {$_z} {$i} {$j} {$k} {$_f}</ArcCW>
<ArcCCW>{$g3} {$_x} {$_y} {$_z} {$i} {$j} {$k} {$_f}</ArcCCW>
<UpperCase>true</UpperCase>
<MinimumArcLength>0.0001</MinimumArcLength>
<MaximumArcRadius>10000</MaximumArcRadius>
<ArcCenterMode>Absolute</ArcCenterMode>
<ArcOutput>ConvertToLines</ArcOutput>
<ArcToLinesTolerance>0.001</ArcToLinesTolerance>
<AddLineNumbers>true</AddLineNumbers>
<LineNumberStart>10</LineNumberStart>
<LineNumberIncrement>10</LineNumberIncrement>
</PostProcessor>

 

[sinebar]

Re: Code issue, please help. This stopped being fun a few days ago.

The attached page is from a Hurco programming manual. I think the last two paragraphs might clear up your problem.




I think your controller is in BNC mode, but your post processor output is ISNC. In that case you'll need to use absolute coordinates for I and J. Or, change the mode of your post processor to BNC.
Does that sound right?

 

[wnec65]

Re: Code issue, please help. This stopped being fun a few days ago.

I took the liberty of loading your program into my Mach3 software And it seemed to run fine. With no tool offset I got a dia. of 1.151 which with a 3/16 end mill would give you a dia. of approx. 1.339. don't know if this was helpful.

 

[ecdez]

Re: Code issue, please help. This stopped being fun a few days ago.

FINALLY!!

I just came in from outside and I owe you guys some drinks! Not sure what change did the trick but the cut is exactly to size and no more pac-man. I'll try to run the full part soon and make sure there's no other issues.

Jim, thanks for you effort with the post. I just couldn't get it to load in the way you recommended so I entered most of it in line by line. If you have CamBam then you're familiar with what I'm talking about; turns out it's pretty easy to modify. I had to eliminate some of the comment stuff as the Ultimax doesn't care for them very much but everything else seems to have worked.


sinebar, I did change it to absolute so that may have played a part too.


wnec65, that was helpful to confirm one of my findings. The coordinates work fine for me in Mach3 too. Helped me to eliminate my vector file as the culprit.



As a side note. I posted this thread on another forum that is exclusive to CNC machines on the same day as the post here and only got 1 response. You guys jumped right in and helped a guy out and I really do appreciate it. Living up to the tagline "The Friendly Machinist Forum"

 

[Marco Bernardini]

Re: Code issue, please help. This stopped being fun a few days ago.

Not sure what change did the trick but the cut is exactly to size and no more pac-man.

Uhm… I just called your CNC machine and told her: «In the next 5 minutes on that table there must be a precise piece… or your gears. Up to you to choose.»

:roflmao:

 

[ecdez]

Re: Code issue, please help. This stopped being fun a few days ago.

Uhm… I just called your CNC machine and told her: «In the next 5 minutes on that table there must be a precise piece… or your gears. Up to you to choose.»

So you made her an offer she couldn't refuse.




Appreciete the phone call :lmao:

 

[ecdez]

Re: Code issue, please help. This stopped being fun a few days ago.

Looks like I celebrated a little too early. I ran the code that night and it came out perfect. Just came in from trying to run a different program and my part has some weird cuts. I reverted back to the file that worked to check myself and now it doesn't cut right but I can't remember if I saved over it or not. In my frustration I made a simple file to cut a circle (again) to check everything and weird cut again. The problem is no where near the problem I had previously but definitely there.


Just when I was getting over my regret of buying this thing I'm back to square one. I checked the post I altered and everything seems to be in order.



Now on to my request. Below is the code I generated for the test circle. Can someone run the coordinates and see if they get anything besides a perfect circle? I got nubs (don't know the proper term) at the 12 and 6 o'clock position. The part I was trying to cut has multiple arcs in it and it appears they all have something screwy going on. I'm thinking it's the post but it worked a few days ago' why not now? At first I thought I closed it without saving but I went through line by line and everything matches my notes. I need to narrow down my search for the problem. If the code, or coordinates generated by the code, is problematic for someone else then I know where to start.


%
N10 G70 G17 G40 G90
N20 T1 M6
N30 G0 Z0.125
N40 S2500 M3
N50 G0 X0.5707 Y1.6711
N60 G0 Z0.0625

----- coordinates for circle cut are here -----
N70 G1 Z-0.06 F6.0
N80 G2 X1.9965 Y1.9547 I1.3118 J1.6711 F17.0
N90 G2 X1.5954 Y0.9864 I1.3118 J1.6711
N100 G2 X0.5707 Y1.6711 I1.3118 J1.6711
--------------------------------------------

N110 G0 Z0.125
N120 M5
N130 M02
E





I'm ready to do one of these :whiteflag: and part the machine out. Not really, but I am frustrated. It was a toss up between this machine and a Tormach. I've been thinking for days that I made the wrong choice. Nice heavy duty small industrial machine but 30 years old and zero support other than the forums. There's something to be said about setting up a new machine and your cutting parts in a few hours. I've been trouble shooting for two weeks.

Sorry for the vent.

 

[JimDawson]

Re: Code issue, please help. This stopped being fun a few days ago.

I loaded your code into CamBam and it looked a little strange until I generated the tool path, then it became a circle. This time the code looks good, the last code was a series of arcs but with different centers.

I am beginning to wonder if the is something wrong in the controller, maybe a noisy comm signal or something. Can you load the full program into the controller and edit it, or at least look at it?

 

[ecdez]

Re: Code issue, please help. This stopped being fun a few days ago.

The screen on the right is burnt out so I can't see the graphic but I'm not even sure that was possible for drip feeding anyway. It might have been only for programming on the controller.

The left screen works fine and that's the one that displays the code for the controller. I believe I can edit it too. What should I be looking for?

 

[JimDawson]

Re: Code issue, please help. This stopped being fun a few days ago.

I would just look for any differences between the original code and what is displayed on the screen. It may be the same, so it in that case, no problem.

I would also try to manually enter the code into the controller and see if you get the same result.

I am asking these questions to try to isolate where the problem is being generated, in other words, is it the controller or the code? In this case the code looks fine, but does it need to be tweaked to run on this controller?

EDIT:

If your controller has a ''conversational input'' function, see if you get the same odd hole shape when the code is generated that way.