Calypso CNC User Forums

happy to report after reloading again that almost everything is right..

i still have only 1 maybe two issues...

the extra cycle start to get to the tool change position when next tool is called. (still need to run a complete cam file)
there was an option in my cam software called manual tool change, i checked the box but have not yet fully tested to see if it fixed this problem

2. soft limit warning

test cam file is loaded
i put in T1 (probe)
probe the stock
regen toolpath
hit cycle start
i immediately get a soft limit warning on Z max . with option to continue yes or no
if i choose yes the program continues to load first tool
but it goes all the way to Z max
then lowers to the TCP i have set ..which is about .5 inch below z max..my soft limit is .3 below z max

i have safe Z disabled
any ideas
rick

Hi,
re extra cycle start: I do not know why you see that; I have never experienced that myself and have not had any other report of this. I think to track this down you will need to start with simple tool changes invoked from MDI.
Do a T# M6 (where # is any tool number that is different than the current tool number already mounted).
That should get you a simple MSM tool change sequence - see if that takes one cycle start or two.

Re soft limits warning: Look carefully at the soft limits settings. D you have the slow zone set large enough that it covers the TCP position?
You can test by using MDI: G53 Zxx where is the value you want to go to in machine coordinates.

Dave

sorry dave... been super busy.... i know your busy too..thanx for the rresponse..

i believe you fixed one already... i know for a fact that the slowzone does not cover the tcp position... i will check change and test that tomorrow morning
i have the feeling the extra cycle start during tool changes has something to do with the slowzone or softlimits for the z (im not sure)

will report tommorow morning...

btw i made some beautiful parts today .. thanks for what you do man

rick

yeehaa the soft limit warning is gone..i couldnt wait till morning,,,

but i still have an extra cycle start before it goes to the tcp position... intead of just going Z to the tcp position...it goes all the way up and hits the limit switch and stops there...then the cycle start makes it go down Z to the tcp position and the x and y follow as well.. its going to z max instead of just the tcp positionZ...

when just do a manual tool change the sequence is correct... i think its really something in the CAM that is causing it.
i had check the M,ANUAL TOOLCHANGE box in the cam to see if fixed the prob...but that was before changing the slowzone to fix the softlimit warning..

tommorow morning ill uncheck the box and repost the cam without that feature checked and retry..

i shouldnt be going to zmax i wouldnt think.. ..but only to Z softlimit..

as i thought..

the soft limit warning on z max was fixed with your input...

i made the change in the cam but no luck with the extra cycle start thing..

on the first tool change it works right but after that it needs an extra cycle start

probe tool mounted master tool t1
probe stock for zeros
load cam
regen tool path
machine goes to tcp position and asks for facemill (but z goes all the way to z max then drops down to tcp position)
does facing operation


time for next tool...so the z goes to z max and thats where its sits until i hit the cycle start button...
i hit the cycle start button...
then machine goes to tcp position

if i just manual tool changes with mdi command then it works perfectly every time...
only difference is that when i use mdi to invoke a tool change the z only goes up to the tcp position i set...
during a part cutting cycle tool change the Z goes all the way up to Z max(hits the limit switch) i think this is what is interrupting the tool change sequence and requiring another cycle start to get the sequence started again..

What type of motion device is being used to drive the machine?
Parallel port? Smooth stepper? Something else?

parallel port

Very odd.
Since you say that an MDI M6 works as expected, that tells me that the MSM M6 scripts are working OK.

Therefore I'm suspicious of the code being created by cam post processor.
What is the CAM program and what post processor is selected?

Can you make a small (and I mean as small as possible as I can't wade thru a complete CAM program output to look for clues) gcode test case file that cases the double cycle start problem on your machine?
Perhaps use the cam system to post a program that does one tool change but not cutting motions?

Dave

i suspect you are correct about the post ...
im using autodesk inventorhsm
for the post processor, i have selected generic mach3 mill

on the following post.... for the first tool change /// facemill ...the tool change does not require an extra cycle start
but for the second op..the centerdrill ... it does require a second cycle start

whtever it is, its in this code... it may just be something i have to live with... although its a bery small thing...because the post work flawlessly with mach3... and msm except maybe this little hiccup

(1001)
(T7 D=1.9685 CR=0. - ZMIN=-0.01 - FACE MILL)
(T17 D=0.25 CR=0. TAPER=90DEG - ZMIN=-0.04 - CENTER DRILL)
G90 G94 G91.1 G40 G49 G17
G20
G28 G91 Z0.
G90

(FACE1)
M5
M9
T7 M6
S1800 M3
G54
M8
G0 X10.1378 Y-0.25
G43 Z0.5906 H7
Z0.1969
G1 Z0.1919 F20.
G18 G3 X9.9409 Z-0.005 R0.1969
G1 X9.8425
X-0.9843
G3 X-1.1811 Z0.1919 R0.1969
G0 Z0.1969
X10.1378
G1 Z0.1869 F20.
G3 X9.9409 Z-0.01 R0.1969
G1 X9.8425
X-0.9843 F15.
G3 X-1.1811 Z0.1869 R0.1969 F20.
G0 Z0.5906
G17
G28 G91 Z0.
G90

(DRILL2)
M5
M9
M1
T17 M6
S1800 M3
M8
G0 X1.204 Y-0.1666
G43 Z0.5906 H17
Z0.1969
G98 G81 X1.204 Y-0.1666 Z-0.04 R0.1869 F5.
X3.4706 Y-0.1722
X5.8065 Y-0.1776
X8.1089 Y-0.1714
G80
Z0.5906

M9
G28 G91 Z0.
G28 X0. Y0.
M30

Hi,
Ok I think you are seeing a post problem....

Here is the 1st tool change snippet of Gcode -

1hander wrote: (FACE1)
M5
M9
T7 M6

For this tool change you only need one cycle start - and that cycle start is what continues the M6 sequence after you have changed the tool.

1hander wrote: (DRILL2)
M5
M9
M1
T17 M6

In this tool change snippet, the post processor has inserted an M1 code. M1 is "optional stop" - which requires a cycle start press to continue after the M1. Then the M6 is executed and that is the "2nd" cycle start press.

I think you said that you selected "manual tool change" as an option in the post processor. I bet that the post is inserting the M1 so that the program will stop there, the assumption being that you then change the tool and press cycle start to go past the M1.

Two solutions:
1) turn off "manual tool change" in the post processor so that the M1 codes are not inserted before each M6 tool change.
2) go to the MSM Run page and turn off the "M1 Stop" Button - that will prevent mach from stopping at an M1 code.

Dave