Inventables Community Forum

[gcode import] estlcam

Continuing the discussion from [new feature] G-code sending through easel:

Can you post the gcode you exported? Do you know if it supports post processors? Here is the spec for what Easel needs

1 Like

Hi,

I can add a preset for Easel to Estlcam.
Can you post a short example how the g-code files should ideally look like (especially the headers / footers)?
What are the default length and feed units?

Christian

2 Likes

Great! The spec specifies the gcode commands that can be used, but in terms of headers and footers the short of it is basically to put as little / nothing as possible. You can write units (G20 / G21, the default is MM) and G0 / G1 movements (G1 must be accompanied by F feed). And avoid putting in any specific initial XY position (like don’t send the machine to X=0 Y=0 unless you plan on cutting there).

Easel supplies the spindle control (although you can also set the specific spindle speed if needed through M3 SXXX) at the beginning and end. Here is the actual output from the easel post processor from Vectric:

G20
G0X2.7292Y-0.0288Z0.2000
G0Z-0.2092
G1X1.2661F50
G1X1.2427Y-0.0105
...
G1X1.3447Y5.5587
G1X2.6553
G0Z0.2000

I’d be happy to add a link to it from Easel. If you could provide a short sentence on how to install / use it, that’d be perfect.

Hi,

can you test the attached file for me?

Easel test.nc (225.7 KB)

It should look something like this:

  • I’ve replaced G2 / G3 with G1 interpolation (this may cause the machine to slow down if Easel uses GRBL)
  • Length unit is mm
  • Feed unit is mm/min
  • There is a tool change included before the outer toolpath
  • file extension is .nc

Christian

Almost! 2 things:

  1. Even if there is a default, I think you should always write a G20 or G21 depending on the units, it is best not to depend on anyone else for that.

  2. You can’t do tool changes. You’ll need to export in two separate files for that.

Hi,

just uploaded Version 8.208 at www.estlcam.com with a preset for Easel:

  • Added G20 / G21 (will switch automatically depending on selected unit) and G94…

Here are 2 example files for quick testing:

  • Example_millimeter.dxf (10.7 KB) Unit of this file is mm / total size: 100 x 100mm / ~4 x 4"
  • Example.e8 (34.4 KB) Same thing but as Estlcam project file with finished toolpaths:

Once you click “File” -> “Save CNC Program” for the first time this dialog box will appear:

Here you can select the “Easel” preset and also change units for g-code output if desired…

If you want to change things later you can do this in the setup tab:

This is what the CNC program should look like:

Tool changes unfortunately can’t be suppressed - at the moment it will create a M5 / M0 / M3 sequence - so it will at least stop the program (no tool change in the example file).

Christian

1 Like

I don’t know what the NC file does, and if it has tool changes. But the line it’s failing on is G00 Z5.0000 That should be support, does it work with G00 and G01 instead of G0 and G1 ?

Version 8.208 will output “G0” instead of “G00” as soon as “Easel” has been selected (see picture above).

I just exported a V-Carve from Estlcam, and imported it into Easel no problem, at least with the G-Code side. I did this multiple times. I think I did find a bug in Easel, I just need to get the case down better before I do the report.

Sorry for sounding thick, but how do you

A) Export from estlcam and B) import it into easel?

Estlcam has an Easel preset:

(I’ve never tried Easel myself - if someone experiences any issues just let me know and I’ll take care of it

Thanks Christian,

But what I mean is that if I wanted to cut out the knife block soldier for example, i go through the steps in estlcam, setting up pockets, cut depths and built up my toolpaths, is that then Exported as a file and imported into easel for it to cut?

hope that makes sense.

Yes - you just save the CNC program (“File” -> “Save CNC Program”) and then open this file in Easel.

By the way: Estlcam also has a integrated controller that should work well with the X-Carve hardware, too

This post was flagged by the community and is temporarily hidden.

@Lim1 what is this file?