how to avoid G02 and G03 in the final g-codes.

[msm19b034]

how to avoid g02 and g03 in the output g-code but replace them with g01 linear interpolation rather than having circular interpolation, we use small chords and cut linearly to get a curvature, so we need to avoid g02/g03.

[seth.madore · Accepted solution]

In some toolpaths, just turning off "Smoothing" would do what you're looking for. Otherwise, a simple post processor edit will get that for you.

What post processor are you using?

[msm19b034]

we use grbl post processor, what settings should i edit while post processor

[seth.madore · Accepted solution]

In the post processor:

allowedCircularPlanes = undefined; // allow any circular motion

Set "undefined" to zero (0) will disable all arcs.

From the manual:

 

[engineguy · Accepted solution]

@msm19b034 

If you are just doing fairly simple cutting along lines around a shape then you could try using the 2D Trace toolpath, it will output in very small linear (G1) moves, no G2 or G03.

See attached image of a circular toolpath that has no G2 or G3 programmed moves, also attached Fusion example file and .nc file.

  Also, depending on the Post Processor you are using that could may be be modified 🙂

[msm19b034]

I don't find allowed circular planes option in the to give it 0. i have attached an ss please show it to me there.

[seth.madore · Accepted solution]

It's in the POST PROCESSOR itself:

You can download the post HERE

 

[seth.madore]

And a tip; only select the post(s) that actually answer the question, not every response 😉

[msm19b034]

now i am in the manufacture module in fusion 360 I clicked actions and pressed post processor, this opens a dialog box where we can choose machine and post the .nc file, now whatever you have shown involves changing the setting in a .cps file, i am asking the procedure how to access the .cps file and save it in fusion for later usage. 

[msm19b034]

the edit option beside post is not enabled is that where you do the changes? if yes, how to enable the option.

[seth.madore · Accepted solution]

Give this a watch/listen:

[serge.quiblier]

Hi @msm19b034 

If it's just for one time, and you don't want to edit the post, you can also edit the values filtering the arcs.

If you changes the minimum arc to 6000, and the maximum arc to 7000, it should remove most of the arcs.

As this will define a filter, "I just want to preserve arcs with a radius ranging from 6 to 7 meters"

Cheers

[engineguy]

@msm19b034 

Looking at this again, grbl should accept G2/G3 code from what I have read.

Just a thought, have you tried setting Arcs Parameter $12 in grbl ?

It should accept the G2/G3 and split them up into tiny lines without any outside help, see below for an extract from the grbl Manual, that is how I read it anyway, could be wrong though 🙂 🙂

$12 – Arc tolerance, mm

Grbl renders G2/G3 circles, arcs, and helices by subdividing them into teeny tiny lines, such that the arc tracing accuracy is never below this value. You will probably never need to adjust this setting, since 0.002mm is well below the accuracy of most all CNC machines. But if you find that your circles are too crude or arc tracing is performing slowly, adjust this setting. Lower values give higher precision but may lead to performance issues by overloading Grbl with too many tiny lines. Alternately, higher values traces to a lower precision, but can speed up arc performance since Grbl has fewer lines to deal with.

For the curious, arc tolerance is defined as the maximum perpendicular distance from a line segment with its end points lying on the arc, aka a chord. With some basic geometry, we solve for the length of the line segments to trace the arc that satisfies this setting. Modeling arcs in this way is great, because the arc line segments automatically adjust and scale with length to ensure optimum arc tracing performance, while never losing accuracy.