// ---------------------------------------- // // The following SmartCAM code generator has been // created to generate NC code for the respective // machine and control combinations listed below. // // Due to differences in programming styles, // controller versions, and optional equipment, // SmartCAMcnc DOES NOT and CANNOT guarantee // that the NC code generated is correct for any // specific machine. Some modification to the code // generator to match your setup and output // requirements is likely necessary. // // Modifications to code generators do not TYPICALLY // require a significant amount of time. SmartCAM // customers with active SMA contracts are entitled // to support for their code generators from the // SmartCAMcnc Support Group. To contact them for // support, please send an email to: // Support@SmartCAMcnc.com. If you would like // information on purchasing SMA for your SmartCAM // products, please contact: Sales@SmartCAMcnc.com // // DISCLAIMER: It is the responsibility of the end // user to confirm and verify that the NC code // created by any code generator is accurate and // will not cause a machine malfunction which // could result in stock, tooling, machine, and/or // personal injury. // // SmartCAMcnc assumes no responsibility or // liability for any damage caused or alleged to // have been caused by the use of any of the code // generators it provides. // ---------------------------------------- @COMMENTS Machine: Cincinnati Milacron Cintimatic VC20 Machining Center with Cincinnati Milacron Acramatic 900 V2 CNC Control Notes: 1. This machine and template file have been set up to support the following fixed cycles: G80 - Fixed Cycle Cancel G81 - Drill Cycle G82 - Spot Drill Cycle G84 - Tapping Cycle G85 - Boring Cycle - Peck Drilling (See note 3) 2. Speeds in the Job Plan should be specified in revolutions per minute (RPM). Feeds should be in inches per minute (IPM). In order to produce code which will turn the spindle in a reverse direction, type the spindle speed in Job Plan as a minus number. 3. For peck drilling the value for the depth of peck can be specified by assigning a value to the variable word #PECK in Job Plan. If you want to peck drill, remember to turn on the peck drill hole operation ( Hole_Op - Peck_Drill) before creating the Hole element and remember to specify the tool as a drill. SmartCAM will automatically output all G0 and G1 movements necessary. If no value is assigned to #PECK in Job Plan, SmartCAM will use the default value of .100 found in question #150 in Machine Define file. When assigning #PECK in Job_Plan, it must be in capital letters perceeded by the "#" symbol. It can be assigned either in the Notes section or the Tool Comment line. Also, a chip breaking cycle may be executed by assigning #U1=1 in the Job_Plan in the same manner. This will cause the drill to stay in the hole, back off .030, then continue with the cycle. If BOTH variables are to be assigned, you MUST seperate them by using a comma. Otherwise, the cycle will not be executed. 4. SmartCAM will output all the necessary moves to turn cutter diameter compensation on and off correctly (G40/G41/G42) but certain rules must be followed in the Shape Module. Any Profile in Shape with an Offset of None needs no Lead_In or Lead_Out moves. All Profiles in Shape with either Offset Right or Left require Lead_In and Lead_Out Lines and may also have Lead_in and Lead_Out Arcs as well. The following procedure is recommended highly: If you wish to use Lead_In and Lead_Out Lines only, it is best to use an Angle of 90 degrees and a Length greater than the tool radius. If you wish to use Lead_In and Lead_Out Arcs, it is best to use a Radius equal to the same amount and an Angle of 45 degrees, then Lead_In and Lead_Out Lines to those Arcs at an Angle of 90 degrees and a length equal to the same amount. Any time Lead_In and Lead_Out Arcs are used, Lead_In and Lead_Out Lines are absolutely necessary. 5. SmartCAM will automatically output the filename as the program number at the beginning of the program. 6. When using Tape_To_Shape, all geometry is interpreted as center of tool. After the translation, it is necessary to change the offsets of the applicable geometry in Shape so that the shape file is a true representation of the translated information. This is done by select- ing Update, Feature_Change, Offset, then choosing the desired geometry on the screen. 7. In order for the tool to retract properly for a tool change, a point must be assigned as the first element in the shape. This point should be assigned the first tool to be used in the shape, with Prof_Top set to No and Clear_Z set to No. Set the Z_Level for the point to the desired Z retract position for tool change. @START % #RESET(#MOV) #ONBLK)MSG,#TLCMT( #EVAL(#U8=#TOOL) #MOVT#TOOLM6 )MSG,( <#FXD><#MOV>#EXLN <#SPNDL> #EVAL(#U3=1) @TOOLCHG ZHOME=#ZHOME #EVAL(#U2=0) #IF(#V5=1) <#DCOMP #EVAL(#V5=0)> #IF(#V9=1) <#FXDR#ZHOME> #ELSE<#MOVZ#ZHOME> )MSG,#TLCMT( #MOVT#TOOLM6 )MSG,( <#FXD><#MOV>#EXLN #IF(#NTOOL<>#U8)#SPNDL #EVAL(#V0=0) #EVAL(#V9=0) @END ZHOME=#ZHOME #IF(#V9=1)<#FXDZ#ZHOME>#ELSE<<#DCOMP>Z#ZHOME> #MOVM30 #OFFBLK @STPROF <#MOV> #EVAL(#V0=1) #EVAL(#V9=0) @LINE #IF(#DCOMP>0) <#EVAL(#V5=1) <#DCOMP><#MOV>> #IF(#DCOMP=0,AND#V5=0) <<#MOV>> #IF(#DCOMP=0,AND#V5=1) <<#MOV> <#DCOMP>> #IF(#DCOMP>0)<#EVAL(#V5=1)> #IF(#DCOMP=0)<#EVAL(#V5=0)> @ARC <#MOV> #IF(#DCOMP>0)<#EVAL(#V5=1)> #IF(#DCOMP=0)<#EVAL(#V5=0)> @ZCLRMV #RESET(#V1,#V4) #IF(#V0=4)<#EXIT> #IF(#V9=1)<#FXDR#ZPOS> #ELSE<<#MOVZ#ZPOS>> #EVAL(#V9=0) @ZCHKMV <#MOV> @ZDPTHMV <#MOV> @FXD1 #EVAL(#V9=1) #EVAL(#V1=#ZCHK-.1) #EVAL(#V4=#ZDPTH+.1) <#FXD> @FXD2 #EVAL(#V9=1) #EVAL(#V1=#ZCHK-.1) #EVAL(#V4=#ZDPTH+.1) <#FXD> @FXD3 #EVAL(#V9=1) #EVAL(#V1=#ZCHK-.1) #EVAL(#V4=#ZDPTH+.1) <#FXD> @FXD4 #EVAL(#V9=1) #EVAL(#V1=#ZCHK-.1) #EVAL(#V4=#ZDPTH+.1) <#FXD> @FXD5 #EVAL(#V9=0) #EVAL(#U9=1) <#MOV> #EVAL(#V1=#ZCHK-.1) <#IF(#V1=#ZPOS)<#UPDATE(#ZCHK)>Z#ZCHK> #EVAL(#V4=#ZDPTH+.1) #EVAL(#V7=#V4+#V1) #EVAL(#V2=ABS(#V4)/#PECK) #IF(#V2<>INT(#V2))<#EVAL(#V2=INT(#V2)+1)> #REPEAT(#(#V2))<#CALL(PECK)> @PECK #EVAL(#V1=#V1-#PECK) #EVAL(#V3=#V1+.03) #IF(#V1>#V7) #IF(#U1=0) #IF(#U1=1)Z#V3> #IF(#V1<=#V7) #IF(#V1=#ZPOS,OR#U3=1)#ELSE> @