Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: SteelWolf on October 12, 2012, 08:49:32 PM
-
Hi,
I'm using Mach3 3.042 and Mastercam X5 with the MACH3GENERIC.PST post.
I setup a custom machine like my Router with portal like axis hirachy and a rotary A axis (along x)
Everything works fine but Mach3 is unable to jump opver the 360 degree. It always changes direction and moves back to 0 degree (destroying my workpiece).
How can I change the post or what do I have to do?
PS: It also slows down my x axis movment drastically like to <1%
I hope someone is able to help me with this.. I tried the last few days but had no success :/
Thanks!
Max
-
Hi Max,
if you want an angle greater then 360 degree then UNCHECK the " ROT 360 rollover " and " Ang Short Rot on G0"
in General Config menu. ;)
Alex
-
Hi,
Thank you for the fast reply!
But think the problem is somewhere else :/.. I tried all this options but it won't affect the result.
Y.006 A-7.612
Y.005 A-6.013
Y.004 A-4.453
A-2.928
Y.002 A-1.446
Y0. A-0.
Y-.002 A-358.554
Y-.004 A-357.072
A-355.547
Y-.005 A-353.987
Mach3 simply doesn't know that it has to jump from the Y0. A-0. to Y-.002 A-358.554 because there is no indicator for the direction it should move I guess?
Can this even be solved within mach3? if no..
Im pretty new to post editing, how can I change it?
Another post problem is that the Z-Axis won't go up before every toolchange..
Greetings,
Max
-
Mach3 simply doesn't know that it has to jump from the Y0. A-0. to Y-.002 A-358.554 because there is no indicator for the direction it should move I guess?
What are you expecting it to do? The code is telling it to move from A0 to A-358.554, so it's going to rotate -358.554 degrees. If you want it to move the other way 1.446 degrees, then you should program A1.446.
If the next position is greater than the current position, then it will move in the positive direction. If the next position is less than the current position, it will move in the negative direction.
-
I didn't want to offend mach3 ;) of course it can't know
But this is the output from the post.. so how are other machines supposed to handle this data? there are about 300 rows so editing it manually isn't an option :/
How can i solve this from the mastercam/postporocessor side?
-
I didn't want to offend mach3 Wink of course it can't know
It knows exactly what the g-code is telling it to do. If you want it to do something other than what the g-code says, then of course, it can't know that.
You didn't answer my question, but it sounds like you want it to move 1.4°. not -358°??
You need to learn how to use MasterCAM better.
-
Hi,
when the code is really correct until the "Y0. A-0." I guess there is a issue in the post processor.
Try using a fanuc PP.
just a thought
Is your A axis turning the same direction as in Mastercam?
Is there any G91 in your code?
Alex
-
IF in Gen config IF you turn OFF all the options under rotation (uncheck) then mach3 will run your code exactly as it is posted.(Just tested it) NOW if it is post wrong then YOU will have to work that out.
As to axis speed you need to go to tool path config and turn on the axis rotation and check use radius for feed rate. THEN on the settings page input the radius of the piece you are working on.
That will sync your axis feed rate to the linear axis feed rates
(;-) TP
-
Hi,
many thanks to all the answers.
@ger21: Yes i want to move only the 1,44° holding my direction.
@cncalex:
No G91 in the post.
The Fanuc post seems to do the trick for the beginning
The code is correct for one revolution, also the direction. after every revolution it returns to "360°" and starts the next one.
Now with the fanuc post (generic fanuc 4x mill) it works but the code is something like:
A-35555.725
A-35558.579
A-35561.422I guess the big angles can't be avoided? The problem is that
I haven't mounted the 4th axis yet so I can't test it but in the preview screen of mach3 it still shows a wrong result where small spherical substractions on cylinder are stretched across the surface like Z axis wasn't fast enough.
There are also some lines like:
X96.812 Y.001 A-1170.004 F3.8
And I have no idea why it would slow down to 3.8? The Z axis movement isn't affected.
@ BR549 & CNC Alex
Only when I turn off all the rotation options I see a decent preview screen but high A axis values.
When I turn on the Rollover , I don't see the rotation of the A-Axis but just X Y and Z movements. (I should attach screenshots..)
Max
-
What do you mean by high axis values the values will be whatever it needs to be to cut the part (;-). IF you are to do continuous 4Th axis movement then the numbers will have to grow very large OR you end up rotating back to zero between each rotation of the 4Th. Some CAMS wrap up the 4Th values to provide smooth cutting then unwrap the axis starting at about midpoint on the program. It saves the time it takes to unwrap the axis between passes.
You need to USE the code on the machine to get the real picture sometimes the MACH3 4Th axis toolpath is not what you would expect to see.
Just a thought, (;-) TP
-
When your A axis rotated 10 times then there should be 3600 degree.
The feedrate in your code depends on your cam settings.
Only when I turn off all the rotation options I see a decent preview screen but high A axis values.
The A axis value that you see is the actual position of the axis in your active work offset ( eg. G54) without cutting the value above 360
when you have a value of let's say 1079 degree, and you check then " Rot 360 rollover " then you see 359 degree but Mach remember the 720 degree (which are cut)
when you uncheck " Rot 360 rollover "
Alex