Drilling op posts differently between 1 or more points

[wdg5555]

If I have two points selected in a drilling cycle it posts like this.

 

G56H2Z3.

M08

Z.1

G94

G71Z.1

G73Z-.625R.1Q.05F10.M54

X-3.595Y.4682

G80 M3

Z3.

M09

 

 

If i have one point selected it looks like this

 

G56H2Z3.

M08

G94

G71Z3.

G73Z-.625R.1Q.05F10.M54

G80 M3

M09

 

 

 

The machine crashed on the secound cycle. Since it did not retract in Z. Any ideas?

 

Using X9 and mpmaster 11.0.06347.

 

 

 
 

[Guest]

typically, that retract callout is redundant....

 

On a Fanuc once it hits G80 that should send it back to it's last rapid height since there's no G99 called

[wdg5555]

typically, that retract callout is redundant....

 

On a Fanuc once it hits G80 that should send it back to it's last rapid height since there's no G99 called

This is for an Okuma. Forgot to mention what machine it was for.

[Colin Gilchrist]

It's an issue with Mastercam with an operation that has a single drill point. The issue is if the NCI File contains the retract point, or not.

 

You can see that with 2 points, you get a "Z3." Move after the "G80". With only 1 point, you dont.

 

There is a post mod you can do to force the Clearance move...

[wdg5555]

It's an issue with Mastercam with an operation that has a single drill point. The issue is if the NCI File contains the retract point, or not.

 

You can see that with 2 points, you get a "Z3." Move after the "G80". With only 1 point, you dont.

 

There is a post mod you can do to force the Clearance move...

Below is the section where I need to change it. I'm not sure exactly how though. I'm assuming gcode$ is a nill value so it skips all of the if statements for the prapidout.

If you could give me some direction I would greatly appreciate it.

 

 

pncoutput #Movement output

if subreps & subout$ = 0, subout$ = 3 #Subrep

pcom_moveb

comment$

if coolant$ <> 0 & coolant$ <> sav_coolant,

[

pbld, n$, sm09, e$

sav_coolant = coolant$

]

if coolant$ = 1, sm09 = sm09_0

if coolant$ = 2, sm09 = sm09_1

if coolant$ = 3, sm09 = sm09_2

if cool_zmove = yes$ & (nextop$=1003 | (nextop$=1011 & t$<>abs(nexttool))), coolant$ = zero

pcan

if cuttype = zero, ppos_cax_lin #Toolplane rotary positioning

if gcode$ = zero, prapidout

if gcode$ = one, plinout

if gcode$ > one & gcode$ < four, pcirout

if mr_rt_actv, #Restore absolute/incremental for G51/G68

[

absinc$ = sav_absinc

mr_rt_actv = zero

]

pcom_movea

[jlw™]

Or you can use ref points in the short term until you can tweak your post.

[Brad Lisle]

_{The code looks fine to me. It's going to do the exact same thing. except for the multiple holes, the tool tip will stay down to Z.1 when rapid traversing between hole locations.}

[wdg5555]

Bump.

 

Is there any problem with forcing a zout move in the pncoutput? Is drilling/tapping cycles the only time the post looks at that section?

[Colin Gilchrist]

'pncoutput' really isn't the best place to do this. You only want the Clearance Plane output after the 'G80'.

 

The best place to do this is in 'pcanceldc$'.

 

Look at the MPMaster post (available on this website) for a good example of how to do this. IHS uses some Parameter read logic to capture if the 'use clearance only at start/end' checkbox is enabled. They also read the parameter for 'number of points in the Drill Cycle'.

 

If there is only 1 point, and the check box is enabled, then they force out the clearance plane.

 

You should be able to Initialize two variables, add the code to capture the data in 'pparameter$', and add the logic in 'pcanceldc$'.