[Uncle Buck]

I'm doing a program Check with a simple taper program...

it's not showing the upper & lower paths...

what switch do i need to turn on inorder to show it?
also in the upper right corner of the screen, where the X,Y,U,V,Z axis co-ordinates are displayed, the U & V are staying at 0...

any ideas? all this use to work before, but i had to reload all my software

Machine is a CX but it should be the same as all mitsubishi controls...

MC Machinery isn't being helpful to me

[Royster]

Sounds like a G code problem to me can you show me some of your code?

[Uncle Buck]

%
L0003/DIE
G90
G92 X-2.0388 Y1.6228
E1040
H1=.0077
F.05
A-0.5 Y1.4202 G41
X-1.8024
Y1.8254
X-2.2751
Y1.4202
X-2.0788
M01
X-2.0188
M01
X-2.0388 Y1.6228 G40
F2.0
G01 Z0.2
E1042
H1=.0066
F.12
A0.5 Y1.4202 G42
X-2.2751
Y1.8254
X-1.8024
Y1.4202
X-2.0388
Y1.6228 G40
E980
H1=.0056
F.25 Y1.4202 G41
X-1.8024
Y1.8254
X-2.2751
Y1.4202
X-2.0388
Y1.6228 G40
%

[stiv_z]

If you are executing the program with the "plot" auxillary function turned on the taper will not be in effect.

[Royster]

Right I think I've solved it:

You don't have any Z Heights in your program (I suspect Z1,Z2 and Z5 on work piece setup page are all at zero)

Your NC would benefit from the following:

%
L0003/DIE
G90
Z1=9.000 (Or your chosen Z height this is the Pivot point of your geometry)
Z2=4.500 (Where Adaptive control measures itself)
Z5=0.000 (or bottom of job, Not important on 2 axis taper but why chance it)
G92 X-2.0388 Y1.6228
E1040
H1=.0077


*NOTE* Z1 and Z5 are usually swapped in 4 axis!

Hope this helps. If your post processor does not output these extra codes you will need to manually edit your NC every time you need to cut non-parallel jobs.

Also have you, since reloading software, performed a wire alignment and taper-Z? If not your taper will not look right.

[Uncle Buck]

in the work piece setup page, the z1 is .8 and z2 is .5 z5 is 0
i'm cutting a 1" thick block and want .2" land then taper...

before the software reinstall all i had to add in to make the program cut a taper was A0.5 and it would shoe up in the program check...

it's a switch that needs to be turned on, i just can't remember which one and MC is not willing to help me out...

i did do the wire align and taper z after the reinstall...

[Royster]

In that case try going to Machining Data, turn over the page and turn on Z1/Z5 display and also original locus?

[Uncle Buck]

in the program check screen i pressed *(astriks) & input and now it works as it should...

read the manual a bit and the astriks brings over the z values and it works good now...

just finished cutting the first taper, came out great!

[Royster]

That's good news, glad all's ok again