Under such scenario I would go to Geo Edit , add a lead-in line to the starting point and give it a line-offset match . Be sure to give the starting point room enough for tool clearance...usually 1/2 diameter + whatever. You may check the Tool Property Change section and click on whatever offset to allow cutter comp.........Laurence Elie, Manufacturing Engineer, Norse Dairy Systems, USA -----Original Message----- From: Vance [mailto:[EMAIL PROTECTED]] Sent: Wednesday, December 05, 2001 2:27 AM To: Mark; mfg-smartcam@kosh. Subject: Re: [mfg-smartcam] Cutter comp
I have been coding tool center in the past because I have't been running much in the way of mass production, the machine is more predictable and I get less cutter comp interferance alarms. I am now ready to try using more cutter comp programming so I can code once and adjust for reground cutters in the tool diameter setting. This group is great! I didn't realize how much help was available. Thanks to everyone! Vance, Q&E, Inc. ----- Original Message ----- From: Mark <mailto:[EMAIL PROTECTED]> To: [EMAIL PROTECTED] <mailto:[EMAIL PROTECTED]> Sent: Tuesday, December 04, 2001 7:49 PM Subject: Re: [mfg-smartcam] Cutter comp Vance, Is this a particular scenario, for turning the cutter comp on early, or routine programming..... Just wondering, because the Haas control seems to have pretty generic (good) behavior. when it comes to cutter comp. Outside of Bridgeport and maybe some early Dynapath controls, I don't recall much need for cutter comp tricks.....( turning on before 'Z' approach') based on centerline programming, as suggested earlier... You should be able to plunge a point in the pocket and feed to the profile (turning comp on) as long as that point is more than half the diameter of the tool away from the profile. Usually if a profile is cramped for space, I will put a " no positive comp allowed" in my instructions, and all should fly... Most cutter comp needs should be handled, in my opinion, with the template file. Let us know if this is a special situation, or, if you normally code "part profile" vs " tool center", which definitely would make most machine controls less tame, in my opinion... (Ex: inputting .+498" vs -.002" as comp. for a 1/2 end mill) Thanks, Mark How can I get SmartCam 11.5 Production Milling to output code with cutter comp to initiate before the first move in Z before starting a profile. For example; entering a pocket which is not much bigger than the diameter of the end mill. (Using a Haas VF-0 vertical machining center) Can I do this in Machine define, or is there an edit in the .tmp file I can make? ====================================================================== To find out more about this mailing list including how to unsubscribe, send the message "info mfg-smartcam" to [EMAIL PROTECTED] ======================================================================
