Hi Steve,
Thanks for the reply. I was able to spend some hours last night on this and found a couple of posts, Fanuc 6M and Fanuc Mill and tried posting using them instead of my modified Mach 3 post. They did manage to get rid of the redundant Z depth and Feed rate call outs, so I examined the actual post processors and figured out using ### in stead of zeros gets rid of a lot of following zero’s, and changing a few “ModalNumber” to “NonModalNumber” got rid of the extra feedrate calls.
I’m using a Milltronics Centurion V control, uses “normal” g-codes and is probably most similar to a generic Fanuc post… it has some extra g-codes that do some other functions, but Fanuc gets me close. Not sure about your software, but any Fanuc, Fadal, Milltronics, and most other industrial processors that I have run into you don’t need an I, J, or K posted on the G02/03 line if the value is zero. For example a circle on 0,0 would look like this:
G00 X0 Y0
G01 Z-.5 F10
X.25
G03 I-.25
G01 X-.25
G00 Z.1
On my G03 line, I don’t need X and Y as it’s a full circle and I have no change in start to end position. No need for a J value as it is zero.
Using an editor, I do, One CNC has a nice free communications and editing software, called oneDNC or NCLink, think one was earlier than the other, but somehow I have both, like the NCLink one better. I do a lot of editing in that now, but it would be nice to have the post do as close to correct as it can, any manual editing I do is bound to be prone to errors, so less is better.
Likewise, re-posting in the shop isn’t the most productive, I work from a wheelchair and I have my shop computer stuffed into a shelving unit to the right of the machine… use a bluetooth keyboard on my lap, squinting at the monitor… so while it’s adequate for transferring the program back and forth from the machine, it’s a bit frustrating to try to do any real programming or such there. Plus, the whole open the software, modify a value, re-post, then send back to the machine, just to change a depth, a peck, or finish amount on an endmill as it wears is kind of bassackwards in production when you can just change one Z depth, Q amount, or a D value for using G41/42 on a profile pass.
Comments in the program are about 4-5 lines above where the action starts, for example, here is a portion of the unedited program:
N0530 (Operation: Drill, CENTER, T13: 90 degree csk, 0.16 inch Deep)
N0540 G00 Z0.1000
N0550 M09 (Coolant off)
N0560 M05
N0570 G49 Z0
N0580 X-16.0000 Y-5.0000
N0590 (90 degree csk)
N0600 T2 M06 G43 H2
N0610 M07 (Mist coolant on)
N0620 S1500 M03
As you can see, the First comment line is on line 0530, then I have 0540 thru 0580 that deal with the previous tool before I get to line 0590 that actually starts to deal with the tool the comments are about. If I could get the 0530 line to show up just above or below the 0590 line, that would be much more clear.
I am still stumped on my canned cycles, was able to add in the G99 on the first line, think I may even have the G80 showing up after the drilling, got rid of the values I don’t need, like D and V. It would be nice to figure out how to state “if drillz = drillPeck, then post G81” , then this would be close to what I need for G83…. I think… “if drillz > drillPeck, then post G83”. Or maybe it could be just a check box in the drilling portion of Sheetcam as to which canned cycle you want, G73, G81, G82, G83, G85, G86 or G89 and it would have the correct letter values associated with each call… some need peck amounts, some need dwell values.
Brian Lamb
blamb11@cox.net (blamb11@cox.net)
Weimaraner Rescue of Arizona
www.vswc.weimaraner.com click on “rescue dogs”
On Apr 27, 2014, at 1:22 AM, Steve Blackmore <steve@pilotltd.net (steve@pilotltd.net)> wrote:
On Sat, 26 Apr 2014 15:21:38 -0700, you wrote:>First problem, when I post a program, it’s a crap shoot as to wether SC will insert a rapid Z move to R level at the beginning of each tool, sometimes it does, sometimes it doesn’t. Not a huge issue as without it just feeds at the last G01 feedrate all the way down.Put a G0 in your post processor if you need one>Second, when the program calls for a Z depth on the tool, say I’m milling around a contour at Z-.500 (working in inches by the way), the program has a G01 Z-.5 F20 on one line, then followed by XY moves to contour, the problem is it repeats the Z depth on almost every line. This is a big issue, if I decide I only want to go .400 deep, I have to go thru and maybe change 30-50 lines of code, and if I miss just one instance of the Z-.500…. I get a crash… just wiped out a set of expensive hard jaws on my vise yesterday. So… given the Z depth is modal, and there is no need to repeat it line after line unless it changes, can this be edited in the post? Do not post a Z value until it changes?Alter then rerun the CAM much safer and quicker. Alternately use aneditor where you can search and replace a word in all or a section onlyof the file. Notepad++ is excellent, and free. Available here> http://notepad-plus-plus.org/> >Third, it also posts a lot of null values, especially I’s and J’s in my G02/03 lines, I was used to if I, J, or K were zero value, you didn’t input them…. this doesn’t effect anything, just something that creates more to look through in the program.G2/G3 the I’s and J’s are mandatory, they have to be stipulated even ifthey are 0 - its a code error otherwise and controller should stop.>Fourth, I had asked you to help me with using canned drilling cycles and while it kind of works now, it always defaults to G83, peck drilling. Can we define that if the total Z depth and the peck amount are equal it uses G81, spot drilling (or alternately have a check box in SC that lets us define which G-code canned cycle we want)? Then that would leave out the Q value, which is the peck amount, I also found I don’t need a D value. When a canned cycle is called, it also has to have the XY position of the first hole in that line, or it won’t drill, which is what is happening now. Also, if you are drilling just one hole, I use G98 G83 X0 Y0 Z-.5 R.1 Q.25 F10 that has the drill retract to the initial level after the hole. If it is a series of holes, then you need the first line to be G99 G83…… and then you need G98 X_ Y_ on the last line. Also, after the canned cycle has been used, the next line after the last hole has to be G80 to cancel the canned cycle.You don’t say what control program you are using but if you are usingMach3 there may well be a bug in the 1083.m1s file. If it’s not datedAugust 2005 - it’s buggy. If it mentions John Guenther in the changessection it’s broken. If not, edit the post processor. If you need thecorrect 1083.m1s file - ask.>I know most folks don’t use canned cycles and just let SC pump out miles of code in place of canned cycles, but there are too many times I find a peck of .35 needs to be changed to .25, if it’s in a canned cycle, it’s one value to change in the code at the machine. If it’s posted “long hand” so to speak, it’s go into the house, pull up SC, modify the parameter for peck amount, re-post, send back to the shop computer, load to machine…. and as luck always has it, it’s a program I had to heavily modify… which means I have to do it all over again.Again - rerun CAM - FAR less chance for an error or put a copy ofsheetcam on the PC in the workshop.>This kind of falls under niggling, but my comments (tool # such and such, description of the tool) come out quite a few lines above where they should be, could those be put right above the T_ _ call?The comment lines seem to start where that action starts?Steve Blackmore–
.,._
Visit Your Group
Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use
,.,_
