need 5 decimal places

[kendo]

I started thinking about a macro for cutting an angled plane on the top of a block
say I've got a 1x3 block 6" long and I want to cut back and forth in X with a positive Y-Z stepover at the end of each pass.
The slope of the plane is ΔZ/ΔY
The problem arises when the step-up in Z requires more than 4 decimal places
For instance,
If ΔZ is .75"
and ΔY is 1"
and the stepover is .005,
thats 200 cuts in the X direction
and each Z step needs to be .00375
If this is rounded up or down. then the slope won't be true

one thing I just thought of,
what if I round the Z value up and down alternately each loop of the macro, then if the last step is .00005 off, I won't really care about that, and the slope might be "irregular", but immeasurably so. (at least, I couldn't measure it)

These blocks I cut all the time are for vise jaws that have the irregular profile of an aluminum extrusion cut into them. So far I've been using bobcad-cam for this and cutting them on our Tree mill, which lets you input as many decimal places as you want. But I hate using that program and I'm always lookin for a reason to write my next macro.

So waddya think?
any different ideas out there?

[Andre' B]

Just because the numbers on the screen are only displayed to 4 places does not mean that the variables are limited to that.

#100=[0.750/200]
#101=[1.0/200]

G0Y-1.1
#102=-0.7500
#103=-1.0000
WHILE [#102 LT 0.0]DO1
G1Z#102F10.0
G1Y#103
G1X-1
#102=#102+#100
#103=#103+#101
G1Z#102F10.0
G1Y#103
G1X1
#102=#102+#100
#103=#103+#101
END1

The variable #100 will have a value of 0.00375 and if used in a while loop to increment the Z position you will get what you want.

[kendo]

thank you Andre
my macro was finished and I didn't even know it!

[JWK42]

Make sure that your machine can position to 5 places. Your servos may only position in .0001 increments. Just a thought.

[Geof]

Originally Posted by JWK42 Make sure that your machine can position to 5 places. Your servos may only position in .0001 increments. Just a thought.

The specs on Haas machines say +/-0.0001 for positioning (repeatability), worrying about 0.00005 is a bit pointless; do the round up round down on alternate passes.

[Kiwi]

Originally Posted by kendo ...... for cutting an angled plane on the top of a block.........any different ideas out there?

You should be able to use code for XY plane and rotate that plane.
Fanuc G68 'Coordinate System Rotation'

[kendo]

someone would have to really explain to me how to do that.

I've never used G68, because my understanding of it is you can rotate coordinates on a plane, but not the plane itself
The section in the Haas manual seems pretty clear about it and I've never had any use for it

but I did find some chatter on the web about a 3D rotation option for some fanuc controls that allows this

[Kiwi]

Originally Posted by kendo ........I've never used G68, because my understanding of it is you can rotate coordinates on a plane, but not the plane itself....

Rotating the coords on a plane has the same outcome as rotating the plane.
I have never used a Fanuc. Maybe only one plane/coordinates can be rotated at the same time?
With a Fagor, one, two or three planes can rotated at the same time. eg. G49 A30 B10 C5

For a Fanuc try this:
G19 (YZ Plane)
G68 Y0 Z0 R36.87 (Centre of rotation. R = Atan(0.75/1.0)
.....Code......
G69 (Cancel rotation)
G17 (XY Plane)

[panaceabea]

I dont know if my issue is the same or not but I have a bunch of code for 3d pockets to be cut for injection molds that have been generated in mastercam x2 that are 5 decimal place ( 1.99999 and the like) the HAAS controller comments these lines out and says its not a number .

Is there a setting I can change to allow me to run my existing programs?

[JWK42]

Suburban Machinery has a very good CNC Code Editor that will search a very large file and format the different X, Y, Z commands to 4 place decimals.
I have used it for about 12 years and really like it. I think they have a demo version to download and try before you buy it. Google "Suburban Machinery Software" and it comes right up at the top
I don't have any interest in their company other than a satified user.

They are--

Suburban Machinery
3777 Harlow Drive
Willoughby, Ohio 44094
216 951-8974

subsoft@buckeyeweb.com

[Haas_Apps]

You already have a editor that will do what you want. Open X2, then select from the file menu OPEN/Edit External. In the dialog box press the editor button and select MCEDIT then select any file.

When MCEDIT opens select the file you want to modify. Once it is loaded select NC Utils, then select shift. In the shift dialog put 0 for the shift factor and enter 4 for the decimal places. Then select all of the axis you want to modify. Press OK and you should be done.

Originally Posted by panaceabea I dont know if my issue is the same or not but I have a bunch of code for 3d pockets to be cut for injection molds that have been generated in mastercam x2 that are 5 decimal place ( 1.99999 and the like) the HAAS controller comments these lines out and says its not a number . Is there a setting I can change to allow me to run my existing programs?

[panaceabea]

Thanks , I figured it was a simple setting in Mcam that would generate files with the correct number of decimal places .