Integration Utility Kit

Mastercam

---

• CAM System: Mastercam
• Company: CNC Software Inc.
• Website:www.mastercam.com

---

Mastercam to Icam Post Interface Documentation

Overview

The Mastercam Interface Kit is designed to accommodate differences in syntax between Mastercam's and ICAM's post processing languages. CAM-POST can directly process the Mastercam ".NCI" file format. Internally, NCI records are converted directly to an APT standard format. The INPUT_FORMAT definition file variable must be set to MCAM to enable this conversion.

• let INPUT_FORMAT = "MCAM" (same as MCAM3)
• let INPUT_FORMAT = "MCAM1" for Mastercam 9
• let INPUT_FORMAT = "MCAM2" for Mastercam X with CAM-POST V19 and earlier
• let INPUT_FORMAT = "MCAM3" for Mastercam X with CAM-POST V20 (default)

Many NCI records do not have a standard APT equivalent. These records are converted to a record, which can be captured inside the post processor for whatever purpose you desire. The following lines show a typical NCI record and the resultant record in the CL file.

NCI record (two lines)

• 1012
• 1 2 3 4 5 6 7 8 9 10

PPFUN command representation for Mastercam 9

• PPFUN/'1012 1 2 3 4 5 6 7 8 9 10'

ISN command representation for Mastercam X

• #1001:1012,1,2,3,4,5,6,7,8,9,10

Mastercam also supports a "cantext" concept, which allows an integer flag to be added (or piggy-backed) on to motions. These flags can then be used in the post processor for special processing. The cantext value is converted into a PLABEL command. For example, a cantext value of "10" added to a linear rapid motion would appear as follows:

NCI record (two lines)

• 0
• 10000 1. 2. 3. -2

APT representation

• PLABEL/10
• RAPID
• GOTO/1.,2.,3.

Mastercam has slightly different record formats for Mill, Turn and Edm applications. Note that CAM-POST does not support the Edm application format. The Mill and Turn formats however are supported. CAM-POST determines the format in use by the operation code (opcode$) defined on the 1013 record, as follows:

• 1 through 99 -> Mill mode
• 100 through 199 -> Turn mode

With the MCAM1 and MCAM2 formats, tool changes in milling mode are represented by a LOADTL command and tool changes in turning mode are represented by a TURRET command. With the MCAM3 format (default), tool changes are always represented by a LOAD/TOOL command, irregardless of the mode.

Post Processor Commands Conversion

Within the Mastercam kit folder, there is an insert.apt file that contains special commands that control NCI to APT conversion details. This file should not be changed. There is also a kit.mac file that contains the following macros:

LOADTL/$P1* $$ Check for MILL tools on lathes

Only valid for MCAM1 and MCAM2 formats. This macro converts LOADTL commands to TURRET commands if the post is a simple lathe. For mill/turn lathes, this macro inserts an APPLY/MILL command before the LOADTL, if necessary, to switch to milling mode. For all other machine types the LOADTL is processed as-is.
With the MCAM3 format, a LOAD/TOOL is generated for both milling and turning tool changes, and an APPLY/MILL or APPLY/TURN is output if required.

TURRET/* $$ Switch to TURN mode on lathe

Only valid for MCAM1 and MCAM2 formats. For mill/turn lathes, this macro inserts an APPLY/TURN command before the TURRET, if necessary, to switch to turning mode. For all other machine types the TURRET is processed as-is.
With the MCAM3 format, a LOAD/TOOL is generated for both milling and turning tool changes, and an APPLY/MILL or APPLY/TURN is output if required.

PPFUN/$P1'' $$ Ignore unprocessed NCI records

This is a "do nothing" macro that removes unprocessed nci record information from the input APT data stream. Without this macro, GENER would issue a diagnostic that the PPFUN syntax was unknown when using the MCAM1 format.

PLABEL/$P1 $$ Ignore unprocessed NCI cantext data

This is a "do nothing" macro that removes unprocessed cantext data from the input APT data stream. Without this macro, GENER would issue a diagnostic that the PLABEL command is not supported.

Back to top