Dave Engvall wrote: > Hi Al, > I suppose there are really two answers to this question. (a). write > the g-code yourself, tedious but gives you exactly what you want or: > (b) use a cam program that generates arcs with cutter comp. > Oh, specifically with cutter radius compensation, here's what I do: I make the CAM package produce the part outline=tool center, in other words with no offset for the cutter radius. I choose some lead-in and lead-out points that are compatible with the expected tool size, and cut all the part outline points with the lead-in and lead-out points as one contiguous series of moves. I then manually edit in the G41 and G40 at the appropriate places. I can then run the program with a 0 diameter tool in the tool table and it will draw the part outline with a ballpoint pen in the collet. Then, I put the correct value in the tool table, and it will show me the moves with the tool radius accounted for. It will also detect any errors that the control would complain about in the real run. I can also set the tool diameter oversize in the tool table to make roughing passes using the same G-code file, then reduce the value to make a finish pass. > Your question gives me a nice lead-in to bring up a small problem > within emc. Cutter comp, in emc, was set up to go two ways, assume > the tool table knows the diameter of the tool and uses that ... or > declare the dia of the tool in the cam program and let it generate > the offsets. The cam I use (synergy) takes the second approach. The > programmers for synergy did this with the idea that the cutter comp > within the motion control would accept small numbers in the tool > table to represent deviations in the tool diameter. That is,to > correct tolerances in the part or compensate for tool regrind one > just entered the deviation in the tool table and were good to go. > However emc barfs on the second approach. Everything is fine until > one enters something besides 0.0 in the dia for the tool table. Since > I expect emc to be a very capable program, thanks to the brilliance > and dedication of the programs, I'm surprised that it does not > contain this feature. > > My local approach (read fix) is to declare a zero diameter tool and > then modify my tool table. > > Maybe one of the developers can explain how easy or difficult this > would be to fix/implement. I don't think it needs "fixing". It requires you to select lead-in and lead-out points that do not contain inside corners, and is strict about this. I have gotten it to work fine. Section 20.4 of this document http://www.linuxcnc.org/docs/EMC2_User_Manual.pdf shows how it works. It even has an example section that I wrote about how to use it. I have not used G41/G42 recently, so it is possible something has gone wrong there, but not likely. This stuff is hard to get right the first time, but once you have made it work a couple times, you will know how to approach it.
Jon ------------------------------------------------------------------------- This SF.net email is sponsored by: Splunk Inc. Still grepping through log files to find problems? Stop. Now Search log events and configuration files using AJAX and a browser. Download your FREE copy of Splunk now >> http://get.splunk.com/ _______________________________________________ Emc-users mailing list [email protected] https://lists.sourceforge.net/lists/listinfo/emc-users
