MechMate CNC Router Forum

MechMate CNC Router Forum (http://www.mechmate.com/forums/index.php)
-   General - MM Operating (http://www.mechmate.com/forums/forumdisplay.php?f=85)
-   -   G code help (http://www.mechmate.com/forums/showthread.php?t=2678)

lumberjack_jeff Tue 30 March 2010 19:03

G code help
 
In many of the parts I produce, I find that the tool rounds off inside corners excessively. I believe that this can be controlled by G61 and G64.

The odd thing is that the code created by sheetcam doesn't include values for either of these codes. I'm left to conclude that EMC uses *something* as a default.

Given the behavior, I suspect that G64 (maintain best speed) is set by default for inside corners, but I'm puzzled why it doesn't do the same thing for outside corners.

Please go easy on me if this is the first sentence of the first paragraph of the first chapter of the book entitled "Don't be an idiot. Before turning on your machine this is what you need to know about G-code."

PEU Tue 30 March 2010 20:37

I don't use sheetcam so I can't be 100% sure, but most cams don't mess with G64, your problem probably comes from some precision setting of the CAM, for example how close a small segment follows and arc or settings like that. Does your postprocessor output arcs (g02/g03) or the output is just g00's and g01's ?

lumberjack_jeff Tue 30 March 2010 21:02

The Sheetcam EMC postprocessor outputs g02 and g03.

Looking through the Sheetcam help files didn't really give me an explanation, but it did give me a partial solution - "overcut corners".
"If this is selected the cutter will cut into inside corners to allow room for a sharp cornered part to fit. For instance if you are cutting a rebate for a square part to fit into this option will save manually squaring out the corners."

JLFIN Tue 30 March 2010 22:46

Jeff,
I recall in a training class in the mid 80's an instructor talking about (this was on a lathe) how when a tool comes up on a corner it is trying to get from pt A to B (around the corner) at the same feed rate as it was traveling, but because of cutter comp it excels through the corner at (a) a faster feed or (b) radius' more of the corner to get there in what it thinks is its aloted time. didn't make much sense to me at the time, or now for that matter, but in everyday practical use I slowed cutter at corners or even had that function built into one of the cam systems i used to own, or, question to you, if you slow down the feed does it still happen? Because that was built into a cam I used to own it makes you wonder if this was common at a high feed. Hope this helps. good luck

lumberjack_jeff Tue 30 March 2010 23:14

Thanks Jim.
EMC has a feed override slider, with which you can adjust the feed speed from 0-120%. Most of the parts I cut take multiple passes. If I adjust the speed between pass 1 and 2, the tool still follows the path of the previous one, so the answer to your question appears to be yes - the exaggerated curves seem to be independent of the actual feed speed - they might be a function of the feed speed in the code however.

Gerald D Wed 31 March 2010 01:12

Quote:
Originally Posted by lumberjack_jeff View Post
. . for inside corners, but I'm puzzled why it doesn't do the same thing for outside corners. . . . .
Inside and outside corners are two different animals as far as a spinning router bit is concerned. For an inside corner, every (mis)movement of the cutter is visible. For an outside corner, the cutter actually has some wiggle room because it goes past the sharp point that you want to create. You can make the cutter move with a small radius around the sharp point and the point will still stay sharp.

bradm Wed 31 March 2010 06:32

The machine has to be in some mode by default when it comes up. As it turns out, this appears to be G64 by default. Check the EMC2 GCode Manual it seems the behavior you want is G61 (or G64 with a rather small P, which is what I generally use). EMC's philosophy on defaults is that since any gcode file can change the machine state, the only safe approach is to specify what you want at the top of your gcode file. Many (Most? All?) CAM systems have a place where you can configure the preamble you want in your gcode files; you should look for that, and place your G61 there - although I recommend a G64 P0.001 or something along those lines instead.

As Gerald points out, the mode is the same for inside and outside corners, you just don't see the inaccuracy on the outside corners.

Oh, and you can see the currently active gcodes on the MDI page (F5)

J.R. Hatcher Thu 01 April 2010 11:29

My Sheetcam program does set G64 or G61. It is found in the post processor you are using. I changed mine from G64 to G61 ........... no more problems with rounded corners.
Brad tell us a little more about G64 P0.001 and what this does? thanks

bradm Thu 01 April 2010 11:56

G61 sacrifices all speed for "perfect" precision, as you know. G64 with a P field sets a "within this precision". So G64 P0.001 in a machine operating under G20 (inches) would say "slow down enough that you make no errors larger that 1/1000 of an inch", which is very close to G61, but gives a little more leeway to the trajectory planner.

You then make a compromise between speed and accuracy by choosing your P value to your own taste / requirements.

J.R. Hatcher Thu 01 April 2010 20:58

Thanks Brad I did not know about that, I will give it a shot and see what happens. ;)

lumberjack_jeff Thu 01 April 2010 21:05

Spectacular. Thank you Brad! I knew I asked the right guys!


All times are GMT -6. The time now is 20:18.

Powered by vBulletin® Version 3.8.3
Copyright ©2000 - 2018, Jelsoft Enterprises Ltd.