Tooltable Output Problem

[R.M.V.]

Hi,

 

I have a problem with my Tooltable Output.

 

It shows as,

 

%
O0005(CAMERA)
(DATE=JAN,02,2015 TIME=02:20)
(OKUMA-OSP200M)
(T17|5. SPOT DRILL |H17|D17)
(T9|10.5 DRILL |H9|D9)
(T50|10. FLAT END MILL |H50|D50)
(T-50|10. FLAT END MILL |H50|D50)========> Don't need this line !
(T-50|10. FLAT END MILL |H50|D50)========> Don't need this line !
(T-50|10. FLAT END MILL |H50|D50)========> Don't need this line !
(T-50|10. FLAT END MILL |H50|D50)========> Don't need this line !
(T-50|10. FLAT END MILL |H50|D50)========> Don't need this line !
(T-50|10. FLAT END MILL |H50|D50)========> Don't need this line !
(T-50|10. FLAT END MILL |H50|D50)========> Don't need this line !
(T-50|10. FLAT END MILL |H50|D50)========> Don't need this line !
(T-50|10. FLAT END MILL |H50|D50)========> Don't need this line !
(T-50|10. FLAT END MILL |H50|D50)========> Don't need this line !
(T-50|10. FLAT END MILL |H50|D50)========> Don't need this line !
(T41|10. FLAT END MILL |H41|D41)
(T-41|10. FLAT END MILL |H41|D41)========> Don't need this line !
(T-41|10. FLAT END MILL |H41|D41)========> Don't need this line !
(T-41|10. FLAT END MILL |H41|D41)========> Don't need this line !

 

I only need one line of each tool. But i think because i used multiple pass, it posts like this. Can anyone help me with this? Thanks in advance.

[Colin Gilchrist]

Look in your 'pwrtt$' post block. That is where the tool table is written. There should be a line of logic that looks like this:

if tool_info > 1 & t$ > 0 & gcode$ <> 1003, ptooltable

It is the 't$ > 0' condition which prevents that redundant output in your tool table.

 

When the pre-read loop is running and calling 'pwrtt$', MP.DLL automatically signs the first occurance of each tool variable as positive. On every subsequent call to that tool number (at the tool changes), that tool number is signed negative. This is done automatically during the pre-read loop, and normal behavior (tool numbers as signed positive) is restored during NC output processing.

[R.M.V.]

Hi Colin,

 

As you told me, i found this line in my "pwrtt$" post block,

if tool_table = 1, ptooltable

I inserted "t$>0" into this line,

if tool_table = 1 & t$ > 0, ptooltable

and it post perfectly,

%
O0005(CAMERA)
(DATE=JAN,02,2015 TIME=18:40)
(OKUMA-OSP200M)
(T17|5. SPOT DRILL |H17|D17)
(T9|10.5 DRILL |H9|D9)
(T50|10. FLAT END MILL |H50|D50)
(T41|10. FLAT END MILL |H41|D41)

Thanks a lot sir.

[Colin Gilchrist]

Hi Ronald,

 

I'm glad you got it sorted out. I noticed you are posting for an Okuma. If you contact your Reseller, there is a separate "Post Processor Installation" program that is available. This program allows you to install all of the "optional" post processors for Mastercam.

 

One of the posts available is a "OKUMA OSP_P200M 4X" Post Processor. There are a ton of Okuma Specific codes added to this post. It supports Hi-Cut, Hi-Cut Pro, and Super NURBS output, and also has the 'CALL OO88' macro output for dynamic work offsets.

 

It would be worth checking out this post processor, as there are a bunch of switches in the top of the post that allow you to enable/disable output for the different options.

 

[R.M.V.]

Hi Colin,

 

Thanks for the info.