[chris2112]

When I generate a profile with cambam, it uses both standard x,y,z codes, but also I and J codes for arcs. If I only have x,y,and z, then use a g64, my machine (a K2 running mach3) does a nice smooth cut. But when going to and from the i and j codes, it has a stutter.

Is there a code like G64 to smooth this out? If not, is there a parameter in cambam to says - don't use i and J arcs.

[holbieone]

g64 on
g61 off

try turn g64 off before you start your arcs then turn g64 back on

[chris2112]

cambam makes 20-30 arcs or so per pass, and I run 6 passes. So manually editing 250 places seems like a lot of work.

Is there a quicker way?

[holbieone]

i would first make a few edits to see if it works the way you want

for the rest you will have to talk to the cambam guys , the post needs to be edited

[chris2112]

If this is what you meant (below), it doesn't seem to work. Now it stops and starts. Before it just stuttered a bit.

So this is a cambam issue? I'd like to just say don't use arcs, but I don't see how. That seemed to work fine in lazycam, but there were too many other limitations i could not work around.

Here is a sample code section.

G61
N57 G2 X17.7024 Y3.0612 I0.0181 J-0.2493
G64
N58 G1 X17.7244
G61
N59 G2 X17.8125 Y3.0449 I-0.0005 J-0.25
G64
N60 G1 X17.8217 Y3.0414
G61
N61 G2 X17.8382 Y3.0345 I-0.0887 J-0.2337
G64
N62 G1 X17.8401 Y3.0336
G61
N63 G2 X17.9121 Y2.9832 I-0.1052 J-0.2268
G64
N64 G1 X17.9203 Y2.975
G61
N65 G2 X17.9326 Y2.9617 I-0.1771 J-0.1764
G64

[mactec54]

chris2112

Add a feed rate to the end of the I & J lines F20. That is less than your G1---- F30. moves & then you don't need the G61 or the G64, use what ever feed rate that works for your job

A G61 won't help much as you are most likely are going around the corners to fast, G61 is exact stop, so it will stop after each move, & then off at the same speed, & in your case break your tool

G61 Exact Stop Mode
G64 Constant Velocity Mode

[chris2112]

I'm sort of following. I run the program at f50. If I slow it to F20 for the arcs, its not as jerky, but its still there. So 60 or so x,y,x moves with G64 is fine. But going back and forth between arcs and x.y.z is jerky, but the arc itself is smooth.

I'm not sure where to go from here. The jerkeyness makes marks that I need to sand out, which slows me down.

chris2112

Add a feed rate to the end of the I & J lines F20. That is less than your G1---- F30. moves & then you don't need the G61 or the G64, use what ever feed rate that works for your job

A G61 won't help much as you are most likely are going around the corners to fast, G61 is exact stop, so it will stop after each move, & then off at the same speed, & in your case break your tool

G61 Exact Stop Mode
G64 Constant Velocity Mode

[ger21]

Try turning off all the CV options in Mach3, and increase the lookahead to 200.

[chris2112]

I set the lookahead to 200 (from 100). I turned off the CV in the code (I didn't see a setting in mach3). Same result. So CV isn't doing much either way I guess.

I tried playing with the acceleration. I had it pretty slow 12/sec. Going up to 50 makes it worse. Down to 9 makes it better, but the transitions are still there.

Any other ideas?

[ger21]

No, in Mach3, turn CV ON, but turn off CV Feedrate, CV Distance, Stop CV on Angles, and any other CV options in general config.

[mactec54]

chris2112

You can still use the G64 put this at the start of the program But give your corners a slower feed rate

[chris2112]

I still have the issue, its just slower if I slow it down.

I noticed that if I generate a toolpath directly from a DXF, without a tool diameter, then I don;t get arcs. Its when cambam compensates for the tool size that it makes arc.

Is there a way to force the code to avoid arcs?

[ger21]

Can you post the .dxf file.
Basically it appears that Mach3 is choking on all the very short little arcs. To me, this usually indicates a poorly drawn .dxf file to start with.

[10bulls]

Is there a way to force the code to avoid arcs?

Hi Chris,

You *can* avoid arcs... in the post processor definition, there is a property 'Arc Output', which you can set to 'Convert To Lines'. This will force all G2/G3 moves to be replaces by a series of G1s.

However, I really would try to avoid that if at all possible.

If your source shapes consist of lots of small line segments, select them, then use the 'Edit - Polyline - Arc fit' command.
For the tolerance, enter a small value. As a rule of thumb, this is about the size your machine can resolve.
In the properties for the selected polyline there is a 'Number of Segments' value. Hopefully the arc-fitting should reduce the number of segments and your toolpaths should machine smoother and faster.

I would also persevere trying to get CV working...hopefully the arc fitting method above will sort out the jerky movements.
You will need to increase your acceleration... CV doesn't work well if your acceleration is too low.

Good luck and I hope this helps!

[chris2112]

I'm not sure how to tell between a poor DXF and a good one. It looks like anything that I use to make code that has curves makes that switch between tiny arcs and x,y,z commands. Its the back and forth that makes the machine stutter.

It seems to only happen when I generate a tool path before making the g-code.

Here is a DXF file and a g-code of a basic shape. One code is clean, the other is the weird arcs.

I'm not sure how to adjust the post processor. I was hoping for a parameter in cambam to just skip the arcs. I turned down my acceleration when I was troubleshooting another problem. It seems to work better. This issue has always been there with cambam generated files. I could draw the offsets in usinf CAD, but I switched to cambam to get away from that (and to have 3d surfacing0

[ger21]

Yeah, that's a bad .dxf

Try this one. It's not exactly the same, but should run smooth for you.

[chris2112]

Its still got arcs. Every DXF I have is bad I guess, from every program.

Is there a way to get rid of the arcs before the code is made?

Yeah, that's a bad .dxf

Try this one. It's not exactly the same, but should run smooth for you.

[ger21]

You want to have arcs. In the .dxf I posted, each corner is a single arc. In yours, each corner is made up of between 37-45+ arcs or segments. That's why you're having a problem. Your problem isn't Mach3's CV, it your sloppy .dxf you're starting with.

[chris2112]

That may be. But this doesn't explain why I get clean running code if I just trace the drawing, but I get the goofy code when I add a tool offset. I've made DXFs a couple different ways. One way is Visio exported to DXF. I don't know how to make them not sloppy. The files I posted were just basic examples. I'm guessing you did a re-draw. Thanks, but that really doesn't help much on solving the issue.

You want to have arcs. In the .dxf I posted, each corner is a single arc. In yours, each corner is made up of between 37-45+ arcs or segments. That's why you're having a problem. Your problem isn't Mach3's CV, it your sloppy .dxf you're starting with.

[10bulls]

I'm not sure how to adjust the post processor. I was hoping for a parameter in cambam to just skip the arcs

Select the 'System' tab (This is next to the top of the drawing tree tab).

Open up the 'Post Processors' group.

Select the post processor in use.
If you haven't selected a different post in your drawing, select the one labelled 'Default'.

At the top of the property grid section (lower left), click the 'Advanced' button.
This will display all the available options for the post processor.

Scroll down to the 'Options' group and look for a property labelled 'Arc Output'. (Sometimes it can be easier to find items by listing all the properties in alphabetical order using the A->Z button above the property list)

Change 'Arc Output' from 'Normal', to 'Convert to Lines' from the drop down list.

The next time you generate gcode it should not use any arc moves, only G1 line moves.

Did you try the Arc Fitting method? Did that help?
It's usually not a problem of having arcs in your gcode, but have lots of small arc moves (lots of small line moves can also cause problems).

Good luck!