VERICUT Users' Forum

DNGUYEN1

Member

From: KS

Registered: 2005-06-16

Posts: 32

M30

Hi all,
  I have one program that so big and it could not fix in our control, so I have splited  7 segments for one tool, and
our machine Simulation go home when ever program reach to 'M30' . even the program did not have G28
my question is how can I tell vericut to disable  machine home when read the M30 and stay at where it was?

    Thanks
Dnguyen

DNGUYEN1

Member

From: KS

Registered: 2005-06-16

Posts: 32

Re: M30

I tested M30 with  MDI it is fine, but until Vericut Call to the  next Segment (program) machine automatic go home.

    Thanks
Do Nguyen

SergeV

Senior Member

From: Irvine, CA

Registered: 2004-10-08

Posts: 507

Website

Re: M30

In the Project Tree,

Select the branch  Setup: 1  (the first branch below the Project)
in the Configure area below the tree, you have 2 tabs,
Select G-Code tab
Un-check the box for "Initialize Machine/Control between NC Programs"

DNGUYEN1

Member

From: KS

Registered: 2005-06-16

Posts: 32

Re: M30

thank you Serger!!!

DNGUYEN1

Member

From: KS

Registered: 2005-06-16

Posts: 32

Re: M30

Our Mazak 1400  using the G43.1 and it will not read the  the tool length offset (H value) if A and Baxis move the same line with G43.1 code
also 'M30' cancel all the tool high offset, how can I set my machine Sim corresponding to the controler.

   Thanks

SergeV

Senior Member

From: Irvine, CA

Registered: 2004-10-08

Posts: 507

Website

Re: M30

In the control configuration, you can add a condition with G43.1 that if it is with A or B on the line to either ignore the command or output an error.

For the M30, you can add the Macros to cancel the tool offsets. you can copy the macros used by G49 to the M30

DNGUYEN1

Member

From: KS

Registered: 2005-06-16

Posts: 32

Re: M30

Serge,
Could you help me how to add the condition with G43.1?

   Thanks
dnguyen

SergeV

Senior Member

From: Irvine, CA

Registered: 2004-10-08

Posts: 507

Website

Re: M30

Configuration > Control > Save as...
-- save the control to a different name (better be safe)

Configuration> G-Code Processing

expand the State branch
find and expand G43.1 to see all the macros it calls
Select any of the macros below G43.1
with the cursor on the macro, right click, Add/Modify
-- the Add/Modify window will come up
-- there are 4 areas separated by bars
In the area identified as Conditions, select Add
-a new condition was added, under Condition, click in the field to open a pull down list, select A
under the Operator column,  click in the field that says "and", select "not" instead
select Add again, select B and "not"
-- Now at the bottom of the window, select Modify

Now the G43.1 will only call these macros and apply the tool length compensation if there is neither A or B on the same line

With the Add/Modify window still opened, Delete both conditions

in the third section where you have "o Macroname o Variable" Select Macroname
in the text field, remove any text (x at the right of the field)
in the field start typing: err 
-- in the list above, you will see a list of macros with the characters err
select ErrorMacro
in the lower section, Override Text = Error G43.1 programmed with Rotary motions
at the bottom of the window, select Add

Close the G-Code Processing window
Reset
test the changes:
Project > MDI...
NC Block Entry = G43.1A5B4  [Enter]
you should get the following error in the logger:
Error: Error G43.1 programmed with Rotary motions
NC Block Entry = G43.1 [Enter]
-- should not give an error

SergeV

Senior Member

From: Irvine, CA

Registered: 2004-10-08

Posts: 507

Website

Re: M30

don't forget to save your final changes

Configuration > Control > Save

DNGUYEN1

Member

From: KS

Registered: 2005-06-16

Posts: 32

Re: M30

Thank you very much Serge!!! it works like a charm.

  Thanks
dnguyen