Nonpolar Axial milling with mill/turn POST

[Anonymous]

I am trying to program a mill/turn part and do some axial milling for a hex along the axis of the part. The machine I am using is a Ganesh Cyclone with Y axis milling on the main spindle. 

I can't seem to figure out how to get the toolpath to post out with XY moves, instead of XC (polar) moves. I have tried several different posts available, but they all output polar milling rather than XY. What am I missing? 

[Anonymous]

You need to edit post processor, search for "got Y axis" statement and see that it is set to "yes"

[Anonymous]

I checked the "gotyaxis" line in all the posts I have tried, and it is set to true. Still getting polar interpolation output?

[Anonymous]

Well, looks like someone with deeper knowledge of post processor will have to answer this one.

But, I am also curious if your post has "use polar" checked as "yes" in user defined parameters on window that pops up when you click on "post process".

[Anonymous]

I have tried the HAAS Y axis lathe posts, and the "use polar" setting is set to off, and I still get polar toolpaths. 

[Anonymous]

Out of my "expertise" now, sorry.

[Anonymous]

Hopefully someone else can chime in here. Seems to me if you have a Y axis lathe post, and you are doing axial milling, your expected outcome would be XY moves rather than polar XC

[Anonymous]

Another thing comes to mind, clue may be in the title of your post. If your tool is in axial orientation, post is likely using polar mode to avoid cutting below part center line.

Have you tried to orient tool in radial direction, that cannot result in polar output because YZ (G19) plane would have to trigger use of Y axis by post.

Result may look like this;

M (?)

G28 H0.

G19

G0 X1.4 Y.5 Z-.25 C0.

G1 G98 X1. F50.

Y-.5 F30.

G0 X1.4

C60. Y.5

G1 X1.

Y-.5

G0 X1.4

C120. Y.5

G1 X1.

Y-.5

etc

[Anonymous]

I have tried that, and it does post out similar to what you showed, but that is ultimately not what I'm looking for. The axial milling with XY moves is going to be a lot more efficient. 

I'm hoping a moderator can comment here. 

[AchimN]

The millturn posts are using XY whenever possible automatically.
The settings below are used to determine whether the toolpath is in or outside these limits:

var gotYAxis = true;
var yAxisMinimum = toPreciseUnit(gotYAxis ? -50.8 : 0, MM); // specifies the minimum range for the Y-axis
var yAxisMaximum = toPreciseUnit(gotYAxis ? 50.8 : 0, MM); // specifies the maximum range for the Y-axis
var xAxisMinimum = toPreciseUnit(0, MM); // specifies the maximum range for the X-axis (RADIUS MODE VALUE)

Into the post attached i´ve enabled the debug output, so you can use that to find out if the toolpath into your project fits into the given XY ranges of your machine.

You can enable that debug code in your post as well into the doesToolpathFitInXYRange() function.

(C-axis position= 25.342)
(toolpath X minimum= -38.148, Limit= 0., within range= false)
(toolpath Y minimum= -19.935, Limit= -50.8, within range= true)
(toolpath Y maximum= 6.87, Limit= 50.8, within range= true)

[Anonymous]

Thank you for your help. I used the post you provided and the debug section is showing all the X minimum within range=false.

How do adjust the limits within the post?

[AchimN]

Please search for this variable into your post:

var xAxisMinimum = toPreciseUnit(0, MM); // specifies the maximum range for the X-axis (RADIUS MODE VALUE)

and set it to your desired value. Note that older versions of the haas posts had that variable twice.

[Anonymous]

That worked out great. I changed that X value to -1000 and then it posted out with all XY moves.