[Donkey Hotey]

I've got a problem with my Mastercam post. Before I can try to fix it, I have to figure out what a helical move should look like.

This is a simple, helical bore with a 0.5" endmill. It's basically opening up a counterbore for a SHCS.

Here is the output:

%
O0000 (Helical Bore)
N100 G20
N110 G0 G17 G40 G49 G80 G90
( TOOL - 3  DIA. OFF. - 3  LEN. - 3  DIA. - .5 )
N120 T3 M6
N130 G0 G90 G55 X-.1237 Y-.1237 S10000 M3
N140 G43 H3 Z.7 M8

N150 G3 Z.62 R.1749 F40.
N160 Z.54 R.1749
N170 Z.46 R.1749
N180 Z.38 R.1749
N190 Z.3 R.1749
N200 X0. Y.175 Z.25 R.1749
N210 R.175 F12.
N220 Y0. R.0875

N230 G0 Z.7 M9 N240 G91 G28 Z0.
N250 G28 Y0.
N260 M30
%

I know that the Haas wants a negative R value if it's going to track a 360 degree arc. If I read the manual correctly, to use the XYZ method, one of the values has to change. In this case, the move is ending at the same XY but different Z. I get the following error:

Invalid X, Y OR

I changed all of the moves above to be negative R. It still gives the same error. What should the output look like for those helical moves? I'm stumped.

[PBMW]

Send me the file and I'll have a look at it...Emails in the profile

[JROM]

first off all your z values are positive......that's not right
And I think you need an end point for the arcs in x&y.
Just my two cents Good luck

[littlerobb]

You are way brighter than I am but, I have done this before. Move your tool to the center of the pocket, and use a g12 or g13.

Example (maybe)
G0 x0 y0 z.1
G1 Z-.1
G91(incremental)
G12 X0 R Q L(loops) D F
G90(absolute)
g1 z.i

[Andre' B]

You can not do a full 360 degrees with a radius specified arc. The start and end points are the same so there is no way for the control to calculate the center of the arc.
You need to us I J type arcs.

[Geof]

N130 G0 G90 G55 X-.1237 Y-.1237 S10000 M3
N140 G43 H3 Z.7 M8

N150 G91 G3 I-.1237 J0.1237 Z-.08 F40. L5
N170 G90 G3 I-.1237 J.1237 Z-.45 F40. L2

N230 G0 Z.7 M9
N240 G91 G28 Z0

[Donkey Hotey]

From the look of things, it's safe to say that I have to rewrite that portion of the post to output IJ moves. I'll see if I can figure it out. Maybe a post in the MC post forum will net some answers.

I don't know if Mastercam posts all arcs the same way or if there is a special case for doing helical pocketing. My fear is that all arc moves will have to be changed to IJ and I'll hate trying to read the output at the control.

Thanks for all the suggestions guys. I knew this bunch would have an answer.

[littlerobb]

Andre b is correct we can cut 359.999 degrees with an R command but it will leave a little mark.

[Donkey Hotey]

I didn't understand why IJK even existed or why XYZ wasn't good enough--until I tried to solve the problem myself (so I could edit the post). Without declaring the arc center (IJK), you have no anchor for the arc.

Less than 360 degrees, G02 or G03, and there is only one solution. Draw a line between the two points, bisect it, move down the bisector by the 'R' value and you have a center point.

Once it becomes a full circle, the arc center could be anywhere. :withstupi I'm not sure why that wasn't more obvious to me in the beginning.

I'm going to check the post and see if there is a switch to output IJK arcs. I seem to remember seeing that somewhere.

[Geof]

If you insist on doing it the hard way see if you can configure it to output sequential semicircles.

[Donkey Hotey]

That's a very good suggestion.

I have almost zero experience with MC posts and my last programming was Visual Basic for Applications about 9 years ago (and I was not ever that good).

Semi-circles or IJK may depend on how much I can learn from the existing code.

All of these challenges just hone my skills for when I want to do something really cool with the mill/MC/post.

[Geof]

.....for when I want to do something really cool with the mill/MC/post.

When you are using CAM 'cool' is somebody else's cool; namely whoever made the CAM program capable of doing what is considered cool.

When you hand code and do something cool, you have done something cool.

Am I a killjoy.

[Donkey Hotey]

Nah, I wasn't talking about making a cool part. I was thinking along the lines of tailoring the post to my specific machine and needs. To make it do things that it doesn't do right now.

Customizing at that level helps forever. Clever changes are still there but it is done at the next level up from the machine.

I still code the lathe by hand. I don't know how you do it. It drives me bonkers.

[Geof]

.....I don't know how you do it. It drives me bonkers.

But if one is already bonkers it doesn't matter. People have been telling me for years that I am bonkers. First it was because I did not use CNC for my business, then because I bought Haas, then because I did not use CAD/CAM. I am used to being called bonkers; being bonkers allowed me to spend the last 20+ years or so doing stuff I found interesting and now allows me to spend a lot of my time relaxing in luxury. I am a big believer in bonkers.

[Donkey Hotey]

This is totally off the subject but I guess I can hijack my own thread.

I am continually amazed at what people think of CNC programming. I get it all the time from people, "Big deal. You want to be a machinist." They don't have a clue all that it takes to create the most basic part.

I tell them to not kid themselves: "This is computer programming where 'crash' has a very real meaning. Do it right and you're rewarded with good parts. Do it wrong and damage thousands of dollars in machinery or yourself."

They still don't get it. I suppose they have to see an endmill travelling at 1000 IPM to find 'Z1' instead of 'Z1.' to appreciate the difference a missing dot can make.

[zedzero]

My ramping program looks like this....all in metric...10mm cutter 25mm hole



%
O1000
(PROGRAM NAME - CRAP)
(DATE=DD-MM-YY - 25-03-08 TIME=HH:MM - 14:26)
N100G21G17
N102G40G49G80
N104G91
N106G28Z0.
N108G28Y0.
(TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - 10.)
N110T1M6
N112G0G90
N114S1000M3
N116G54X7.5Y0.
N118G43H1Z10.M8
N120Z2.
N122G1Z0.F100.
N124G3X-7.5Z-.5R7.5
N126X7.5Z-1.R7.5
N128X-7.5Z-1.5R7.5
N130X7.5Z-2.R7.5
N132X-7.5Z-2.5R7.5
N134X7.5Z-3.R7.5
N136X-7.5Z-3.5R7.5
N138X7.5Z-4.R7.5
N140X-7.5Z-4.5R7.5
N142X7.5Z-5.R7.5
N144X-7.5Z-5.5R7.5
N146X7.5Z-6.R7.5
N148X-7.5Z-6.5R7.5
N150X7.5Z-7.R7.5
N152X-7.5Z-7.5R7.5
N154X7.5Z-8.R7.5
N156X-7.5Z-8.5R7.5
N158X7.5Z-9.R7.5
N160X-7.5Z-9.5R7.5
N162X7.5Z-10.R7.5
N164G0Z10.
N166M5
N168G91
N170G28Z0.M9
N172G28Y0.
N174M30
%

[Donkey Hotey]

Very interesting. From the tool comment line, it looks like you're using Mastercam as well. Which version? I'm on MCX MR1.

It looks like your post is putting out arcs in 180 degree chunks. I'm going to guess you have a later version of MC and they eventually fixed the post. There is hope.

[zedzero]

Very interesting. From the tool comment line, it looks like you're using Mastercam as well. Which version? I'm on MCX MR1.

It looks like your post is putting out arcs in 180 degree chunks. I'm going to guess you have a later version of MC and they eventually fixed the post. There is hope.

I've got X but prefer 9...it's a comfort thing...will have a look at an mcx set up

check your control definition in Arc>mill>helix support...check in all planes supported

I might be barking up the wrong tree here...I'm not an expert

[Geof]

zedzero's ramping program is doing what I suggested, multiple semicircles. Obviously you can tell you program to do this.

[Donkey Hotey]

Zedzero, you are a genius! Thank you. You found it. It was in the Arc tab of the control definition.

They have numerous tab settings for how Mastercam breaks up arcs, sets the radius, etc. Here is the same helix now:

G3 Z.62 I.1237 J.1237 F40.
Z.54 I.1237 J.1237
Z.46 I.1237 J.1237
Z.38 I.1237 J.1237
Z.3 I.1237 J.1237
X.1237 Y.1237 Z.26 I.1237 J.1237
X0. Y.175 Z.25 I-.1237 J-.1237
J-.175 F12.
Y0. J-.0875

I need to actually verify that this method will run and that it's going in the right direction but that looks like the solution. Thank you again.