Chatter from switching between g1 and g3

[sieg01]

If I cut out a big rounded rectangle... I am getting some sharp stopping and starting with no apparent deceleration) when I am getting to the curvey part of the corner. (It is cutting just great elsewhere).

The rapid starting and stopping around the corner leaves some bumps due everything flexing a bit.

It appears to be happening at the same time it gets in to code that is alternating between g1 and g3...

Example code generated from sheetcam:

N34180 G03 X0.1718 Y2.9035 I0.0622 J0.0057
N34190 G01 X0.1866 Y2.7524
N34200 G03 X0.1867 Y2.7520 I0.0622 J0.0061
N34210 G01 X0.2019 Y2.6068
N34220 G03 X0.2020 Y2.6064 I0.0622 J0.0065
N34230 G01 X0.2177 Y2.4674
N34240 G03 X0.2177 Y2.4669 I0.0621 J0.0070
N34250 G01 X0.2339 Y2.3343
N34260 G03 X0.2340 Y2.3337 I0.0620 J0.0076
N34270 G01 X0.2506 Y2.2077
N34280 G03 X0.2506 Y2.2070 I0.0620 J0.0082

It is doing a bunch of little curves.

Is there any additional processing demand or time delay when it is generating the curves? I am on the edge of specs of EMC (700mhz 128ram).

Thanks!

[Boots]

My question to you is who is doing your drawings and creating all those short segmented lines? this will destroy your machine if you continue this way. These lines are so short that your machine ignors the ramping because it cannot do it. I have the same problems getting some drawings from customes doing work in Rhino and they use Splines. (short segmented lines). I can see by your line numbers (34,280) that is almost laffable. You will have to redraw the part and keep radii full and long so your machine can get up to speed and stop the jerking. (A rounded rectangle? ? ) do you mean an Oval? or are you talkin just radius corners? Just radius corners is very easy to draw and the line count should only be 8 lines to cut the shape. Wow what a difference huh?

[sieg01]

I have been building my machine for the last few months and I just had my first cuts on friday. I have no experience with any kind of cam software. I am trying to learn this on my own... so I don't know what is laffable and what is not. It didn't seem like it was damaging the machine. The only problem is that the finish on side of the board has little bumps from the flex and that it drastically slows down the cutting.

I am doing all the drawing. I am drawing it out in inkscape with just a few points (using some Bezier curves). I import it into sheetcam and that is where I get all the points. It looks like it changes the sharper curves in a a repeating short line and and short curve. It seems to handle it fine everywhere else.


So your saying that between each g0 it should ramp up and then ramp down between each point?? That doesn't make any sense to me... and that is not what I'm seeing even for the points that are far apart where it would have time to ramp up and down.

It isn't just a rounded rectangle or an oval. I am trying to do more complex curves.

Two examples:





Thanks

[Boots]

In CNC Machining every line has a beginning and an end. If you put these ends too close together your machine will suffer greatly. I can see by your code that these lines are way too short. Because CNC machines move large amounts of weight (Head, Gantry, Tooling etc.) they can not start at 300 IPM feed. They have a ramp-up to speed and a ramp-down so they don't go BANG when they get to the end of a line. They all do this. So if your lines are too short for this to happen you get jerky moves and banging and a very rough surface like you say you are getting. Sorry to say your programming is laffable but it is and I wouldn't run my machine in such a manner. Not only is it damaging to your new machine but you'll get poor quality parts and at a Turttle pace compared to what you could be doing it. Also did I mention that this condition is very bad for your tooling too. It will cause it to over heat and dull quickly.
I didn't know this was a home made machine. I gotta give you guys credit though for trying to do this on your own but it's like performing Brain Surgery on yourself after reading a report on how easy it is. You need some help in getting your programs shortened up so they run faster with fewer and longer lines and arcs.
By the way G0 is rapid, G1 is straight line feed, G03 is feed in counter clockwise direction G02 is feed in clockwise direction. I see no rapid moves (G0) in the code you have here. You will also need more Ram if you are going to run programs with thousands of lines.
Those parts look like surf boards or wake boards. How long is your cycle time?

[Boots]

Another thing is that you won't see your machine Ramp up to speed because it's too suttle and fast to see. When your machine receives a command in the line of a G1,G02,G03 (there are others too) it will ramp up to the speed you have programmed until just before the end of the line at which time it will ramp down in feed to make a turn. Your problem is that it runs out of line before it gets up to speed and has to stop and change direction then start the ramping again only to run out of line and change direction again. Does this not make any sence to you? Just asking. Because you might not know about some of these things being you are just getting into this.

[sieg01]

Doh! I mistyped I had meant g1 instead of g0.

I understand the need to ramp up and ramp down... An example to understand better...

If I was cutting a straight line at 100 ipm in my X direction. At a certain point I want to move 45 degrees line (So I suppose that would be about 70 ipm in the X and Y to keep it at 100 ipm). When I come up to the point where the angle starts will it:
a) ramp down the x axis to 0 ipm when it hits the point and ramp up the X and Y to 70 ipm
b) ramp down the x axis to 70 ipm by the time it hits the point and then start to ramp up the Y axis to 70 ipm.




Also. I was messing with flattening the curve to produce much less lines that are straight and not curved in inkscape. I am not sure how to produce nice arcs. I thought the cam software would produce better curves (from the bezier curves) using g02 and g03. But it appears to look very similiar with far less points.

Yes I was working out cutting out kiteboards (similar to wakeboards and surfboards). I have cut 2 and they look pretty good... Just might need to sand the edge when I get all done.

Right now they are just in 2d... I'd like to cut them out in 3d but first I need some more experience in 3d cad.

[sieg01]

I have the acceleration set pretty low so that I can hear the speed coming up. Which, I suppose, would make the problem worse on the small lines.

[sieg01]

It is taking 5-10 minutes to cut a board. I was also doing some pocketing where the foot strap is and that was taking a bit of time.

[Boots]

If you can adjust your acceleration and decelleration then perhaps this is all you need do and just live with the short lines. But if it were me I'd fined a better programming tool. When I draw a curve I tell it where the start point is, the end point is, and the radius I want it to do between the points and the software just does it. I use AlphaCam by Planit it's very nice but $$$$$ I think it's $5,000.00 for level 1 milling. (2D only) You would have to spend about $15,000.00 to get the full 3D for a 3 Axis Mill. It would solve your programming issues but there is a learning curve and it's a lot of money. Here is a free simulator to check your NC code to see if it's correct.
www.cncsimulator.com

[Boots]

On my machine that looks like about a 2-3 min. part.

[Seb]

I think EMC2 should be able to handle lots of little moves fine with the new blending code Chris put in (fewer longer moves is still preferable, but lots of short moves should be doable).

Do you know what path control mode you're using? You may be in exact stop mode or exact path mode, which will slow things down a lot. Continuous mode with an appropriate tolerance setting may be better for you. See the EMC2 User Manual for details.

You might try the emc-users mailing list and #emc on freenode, there's lots of very knowledgable people there who are willing to help.

[samco]

try g64px.xxx where x.xxx is how close you want emc to follow your path.

http://wiki.linuxcnc.org/cgi-bin/emc...jectoryControl

sam