Chris Thank you for the explanation of your application that you are using.
I use somewhat the same method to set up the parts on the machine . I have a touch probe pick up the part and store the variable in the machine. Then when the part programs are run the program calls the stored variable and the part angle is set in the G68 line. Works nice. I did get some training and some coder help from a company in the Twin Cites. On setting up work planes and to be able to code the G68 line and also the code the correct angles for tipping of the head on the 5 Axis machine that I am running these programs on. I am using the from world coordinates to code the point in which to more the G54 offset to the rotate the head. G68 X#XFO Y#YFO Z#ZFO I1 J0 K0 R#FMT(#rindex,D3.4)//(REFERENCE FROM WORLD ORIGIN) Thanks for the responds Brock -----Original Message----- From: [EMAIL PROTECTED] <[EMAIL PROTECTED]> To: Brock Shimon <[EMAIL PROTECTED]> Date: Friday, March 17, 2000 9:17 AM Subject: Re: [mfg-smartcam] G68 ? > > >Brock, > Sorry about the delay. The application I use G68 for is probably different >than what you would like to accomplish, but let me describe how I use it: > I frequently run workpieces that are larger than my machine travel, so when >I have to "spin" it around, I use G68 on the second setup to eliminate having to >"square up" the workpiece (saves time). In the second setup, I pickup two points >that are in line on the print and use these points to establish location and >angle of rotation. These two points are always bored holes. Overall location is >important, so I take the time to "square up" and carefully pickup location on >the first setup. Since I am picking up bored holes on the second setup, an >accurate hole-to-hole relationship is maintained from one setup to another. > To setup G68 on my machining center, I pickup location of the first "point" >and put it's x,y coordinates into the G54 work offset, then pickup location of >the second "point" and place it's coordinates into the G55 work offset. In >SmartCAM, I place a point in the process model in the same location as the first >"point" picked up on the machining center. This point in SmartCAM must be the >same as the first Step in your Process Model, and must be the first Step Element >in the Process Model. I usually insert it as Element "1" to insure this. > The following line is hard-coded at the beginning of my code files: M98 >P9507 >O9507 is a simple Fanuc program I wrote that calculates the "angle" between the >two points picked up on my machining center, and places that value in variable >#507. You could just as easily figure it out on a calculator and manually input >the value into the variable. My way just automates the process (less chance of >operator error). > After every tool change, the following line is hard-coded: G68 X__.____ >Y__.____ R#507 >The X and Y coordinates will be the location of the point inserted in SmartCAM, >the same location as that of the first point picked up on the machining center, >and R#507 references the angle value in variable #507 to establish the angle of >rotation. Now when I run the program, the location and angle of rotation are >established and the machining done on the second setup will be aligned with that >done on the first setup. > >To summarize: >(1) Define a point in SmartCAM that has properties that match the first Step in >your process model >(2) Place this point where you want the center of rotation to occur. It will be >your "pivot" point. Make sure it is the first occurring Step element in the >visible database. >(3) Add the following line to your .tmp: "G68 X#XHOME Y#YHOME R#507" This >variable is in your machining center control, it can be any you choose, or >change the #507 to an angle you wish to hard-code. If you want to use a >variable, input the desired angle of rotation into it (on your machining >center). I saved my .tmp file under a separate name, and use it only for when >axis rotation is needed. >(4) Process your code. >Hope all of this helps. Feel free to ask if anything isn't clear, I did the best >I could to lay it out. > >-Chris > > These are the START and TOOLCHG sections from my .tmp: >@START >#EVAL(#U9=0) >#IF(#U9=1) > % > O0000 (SMARTCAM FILE=#FILE) > M98 P9507 >#ONBLK > G54 > G00 G17 G40 G49 G80 G90 > G91 G28 Z0. M05 > (#TLCMT) > /T#TOOL > /M06 > S#SPEED F#FEED > G68 X#XHOME Y#YHOME R#507 > G00 G90 X#XPOS Y#YPOS #SPNDL > G43 H#LOFF Z#ZPOS #COOLNT > /T#NTOOL > >@TOOLCHG >#IF(#U9=1) >< #FXD> M09 > G91 G28 Z0. M05 > M01 > (#TLCMT) > /T#TOOL > /M06 > S#SPEED F#FEED > G68 X#XHOME Y#YHOME R#507 > G00 G90 X#XPOS Y#YPOS #SPNDL > G43 H#LOFF Z#ZPOS #COOLNT > /T#NTOOL > >--------------------------------------------------------------------------- ------------------------------------------------------------------------ >>Could you send me a copy of a *.tmp & *.smf . >> >>I would like to see one that can code the G68 line automatically >>I have to hand edit it in. >> >>I would appreciate it >> >> >>Thanks >> >> >>Brock > > ====================================================================== To find out more about this mailing list including how to unsubscribe, send the message "info mfg-smartcam" to [EMAIL PROTECTED] ======================================================================
