Archive for the ‘ projects ’ Category

Using Autodesk Fusion 360 with the X-Carve CNC & 3D Mesh

Overview

I’d been stuck on an old Macbook Air for all my CAD/CAM work for the past number of years.  And because of that, I was limited to MeshCAM (no disrespect, I quite like it, but one of the few mac apps for CNC I could find) for all my 3d-mesh carving.  I’d dabbled with Autodesk Fusion 360, but the ol’ Mac wasn’t powerful enough to handle it well unfortunately.

Finally got a new PC, and can start to branch out into other CAD/CAM apps.  I’ve been using my X-Carve CNC for just over a year now, been a great learning experience both with its hardware, and the CAM software that generates the toolpaths for it.  And as much as I appreciate how much I’ve learned from MeshCAM, I felt like there could be a more robust solution, and that’s where F360 comes into play.  I am by no stretch any sort of CNC expert, just an avid hobbyist, but I was really surprised how much the F360 team has put into its CAM solutions.  The below post is an overview on my first steps to get it working, specifically for cutting 3d mesh (rather than parametric solids) so I don’t forget what I did in the future.

I should note though, if you don’t care about cutting 3d mesh, this tutorial is still a valid intro to generating toolpaths with F360.

Disclaimer : Not a CNC expert.  Not a F360 expert.  What I list below are ways I figured out how to do things by looking through the docs, and a lot of forum posts.  There may be better ways out there to do any of this.  If so, please let me know!

Note, I use the term “RMB” a lot below.  That means “RightMouseButton”.

Fusion 360 CAM Docs

These are the docs I got the most out of when it came to learning its CAM capabilities.

And an informative tutorial:

F360 Installation

Really nothing to report here:  Install went off without a hitch.  It should be noted that F360 is cloud-app, meaning everything you do gets uploaded to the cloud.  I remember back in the day when it first came out there was a way around this, to only ever work locally.  I’ve not looked into that recently though.

Importing your mesh

F360’s CAM package can’t deal with 3d mesh natively (at least, I’ve been unable to find a way) : You first need to convert it into a solid it can deal with.  And in this case, it needs converted to a ‘BRep’ : I’ve been unable to actually figure out what the definition of a BRep is, but I’m guessing it’s a (solid)BodyRepresentation.  This process probably took me the most time to figure out, not having a broad knowledge of how F360 works.  The trick is, you can’t have any ‘history’ enabled when you do the conversion : The menu won’t even be there if that’s the case.

Note if you don’t care about 3d mesh, and just want to cut your solids, you can just skip this section.

Prep the mesh for import

Before you import/convert your mesh, you should be certain of a few things:

  • There are no holes in it.  It should be a solid mesh, no non-manifold geometry… quality solid geometry.
  • It should be triangulated:  While F360 accepts quads or n-sided polys, I found that it’s internal triangulation function, which appears to be auto-ran when converting to a BRep, sucks, causing poorly converted mesh. Pre-triangulate your mesh.
  • F360 will complain (but still do the conversion if you tell it to) if the mesh is over 10k tri’s, citing poor performance to BRep’s.  I presume this is for good reason.  Right now, I just auto-downres my mesh via Meshmixer.

Import into F360

These are two solutions I’ve come up with:

Method A

  • From the Model Workspace, access Insert -> Insert Mesh.
  • Browse to your obj or stl.
  • RMB on the root Component in the Browser or the gear icon in the bottom right hand corner of the window: “Do not capture design history”.
  • Once inserted, access the RMB marking menu either on the mesh itself, or via the mesh in the Bodies section of the Browser and -> “Mesh to BRep”:  This creates a new Body.
  • RMB on the root Component in the Browser and “Capture Design History”.

Method B

  • From the Model Workspace, access Create -> Create Base Feature
  • Insert -> Insert Mesh
    • Browse to the mesh on disk, hit “Ok” in the “Insert Mesh” dialog
  • Once inserted, access the RMB marking menu on the mesh and “Mesh to BRep”
  • Finish Base Feature via the top menubar.

The imported mesh:

meshImport

Via either method, at this point you can delete the original mesh from the Browser.

This will now give you a ‘body’ the CAM package can deal with.

f360body

Dealing with scale

Note, that based on where you authored your mesh and the units it was in, you may need to scale it up.  For example, I work in Autodesk Maya in cm units.  I need to scale that mesh up by a factor of 1o either before I export, or once in F360, to get it in mm correctly.

Setting up CAM

First, switch to the CAM workspace in F360.

Manage your tools

Before you can start making toolpaths, you need to tell F360 what cutting tools you have:  Via the CAM workspace, access MANAGE -> Tool Library.

Uncheck all the libraries on the left except “Local”/”My Tools”.  Select “My Tools”.

Press the “New Mill Tool” button on the top bar, and start filling out the info for all the bits you own/want to cut with.

Nice page showing what all the values mean:  “New Mill Tool Reference

But in general the below values are always equal to or less than the one that came before it, from the “Cutter” tab:

  • Overall Length:  Total length of the tool,  say, 2.5″ for a fictional bit.
  • Body Length : How much of the tool sticks out of the chuck, or “Holder” in F360 terms. Obviously variable every time you insert it, but say 1.5″ here.  That leaves 1″ inside the chuck.
  • Shoulder Length:  From the tip of the bit to the last part of the thread, even the non-cutting part of the thread, say 1.25″.  That leaves .25″ between the end of the shoulder, and the chuck.
  • Flute Length:  Length of the cutting surface, like 1″:  There’s .25″ of non-usable cutting surface.

I should also note that with the 1/4″ chuck on the DeWalt611, it has 2″ of internal space for bits.

You can also make “Holders” for your different chucks:  Doesn’t seem necessary, but I did it anyway.

Create a Setup

Setups collect the rules that define the the stock to cut, and the toolpaths to cut in them.

Via the SETUP menu: New Setup : This will immediately open the SETUP dialog.  Below are good defaults I start with, but obviously every situation is different.  I skip over values I don’t change.

  • Setup Tab
    • Setup:
      • Operation Type:  Set this to Milling.
    • Work Coordinate System (WCS):
      • Origin: Selected Point : I pick the point on my mesh in the top of bottom left corner, which is the usual (0,0,0) position for the X-Carve:
      • stockZero
  • Stock Tab
    • Stock
      • Mode : Relative Box Size : This creates stock relative to the size of the model you’re working with.
      • Stock Offset Mode : No additional stock:  The stock is the exact size of the model.

This creates a new Setup for the given solid model.  If you hide the body via the lightbulb in the browser, you’ll see a ghost of the resultant stock:

stockGhost

Create a rough clearing operation

Now that there is a setup which defines our stock and the WCS origin, we can start adding toolpaths.  The order is important, since F360 cuts them in that order in Simulate mode.

Note, F360 has great tooltips, many with pictures:  Hover over the given field and see what pops up.

Via the “3D” CAM button, there are two clearing options available:  “Adaptive Clearing” and “Pocket Clearing” :

  • Pocket clearing is closest to what I’m familiar with in MeshCAM:  It removes material layer by layer, which is good for a light-weight machine like the X-Carve.
  • Adaptive Clearing will attempt to burrow down to the full length of your tool, then start cutting material against the full length of the tool. While this sounds great, I’m not sure how well the X-Carve would handle it, and have yet to test at this point (probably would need to cut very slow…).

Choose the “Pocket Clearing” operation:

  • Tool Tab
    • Tool : Select a tool you defined above.  The below “Feed & Speed” section will be auto-populated with that tools defaults.
    • Feed & Speed
      • Adjust as necessary based on the type of material you’re cutting.  How do you know what to set?  Based on my hobbyist level experience it’s all about learning what others have done, + trial & error.
  • Geometry Tab : Controls what area of the mesh will be machined.
  • Heights Tab:  A nice graphical way to set the vertical areas to be machined, and how far the tool-head should retract.
  • Passes Tab
    • Passes
      • Manual Stepover : If you want direct control over this, you can check this and set the min/max values.  Note that F360 can either use hard-coded values, or expressions for the fields : RMB on the “Maximum Stepover” field and “Edit Expression”:  You’ll see something like this pop up:
        • Math.max((tool_diameter – (2 * tool_cornerRadius)) * 0.95; tool_diameter * 0.20)
      • Change it, edit it, etc, based on your needs.  Here’s an example video on how to do that.
      • Direction : Climb by default, but machines like the X-Carve should have it set to “Conventional”, so the cutting edge bites into the material with the direction of toolhead travel.
    • Stock to Leave:  Here you can set how much stock is left over for the finish passes.  How much should you leave?  I generally make this a percentage of the diameter of the finish bit I’m using.
    • Smoothing : In general it sounds like you want this checked on, check the tooltip.
  • Linking Tab
    • Linking
      • Retraction Policy : I’ve had good success with “Minimum Retraction”.
    • Ramp
      • Ramp Type :
        • If you’re cutting wood, “Plunge” seems good.  If you’re cutting metal, then “Helix” is the way to go.

There are obviously many more options, but the above got me started well.

After you hit “Ok” in the dialog, you’ll see the new Pocket operation in the browser show up : While it’s calculating the toolpath a % value will be visible.  After a few seconds, the toolpath should show up, presuming you have the pocket operation selected.

roughPocket2

 

Create one or more finish operations

F360 comes with quite a few finish operations.  Technically you can use can combine as many as you want, but again, build them in order of operation.  In this example, I’ll use the “Parallel” operation, because it most closely emulates what I’m used to in MeshCAM.

Via the 3D  Menu access “Parallel” operation:

  • Tool Tab
    • Tool : Select the tool for this pass. But default it’ll choose the tool used in the operation before it. Note if you choose a different tool, obviously you’ll need to go through a toolchange operation (which on the X-Carve is a very manual step), and need to save out your gcode as multiple files.
  • Geometry Tab : Controls what area of the mesh will be machined.
  • Heights Tab:  A nice graphical way to set the vertical areas to be machined, and how far the tool-head should retract.
  • Passes Tab
    • Passes Options to control the angle of the surface to be machined, the stepover, etc.
      • I like to set my stepover to be 10% of the bit width to give a nice, smooth finish, which you can set as an expression by RMB on the “Stepover” field & “Edit Expression”:
        • tool_diameter * .1
    • Smoothing : Like in the rough cut, this seems good to check on.
  • Linking Tab
    • Linking
      • Retraction Policy : I’ve had good results with “Minimum Retraction”.

After you hit “Ok” in the dialog, you’ll see the new Parallel operation in the browser show up : While it’s calculating the toolpath a % value will be visible.  After a few seconds, the toolpath should show up, presuming you have the parallel operation selected.

parallelFinish

Like mentioned above, you can add more finish passes using different techniques here as needed.

Name your setup and operations

It’s a good idea to name your setup and operations, so you know what you were up to months later.  Click once on a name in the Browser, then click again after a second: It’ll let you rename them:

passNames

Save operation templates

Presuming you get values you like and want to resuse thes on other cuts later, there are two ways to access the data:

  • You can open a previous cut, then RMB on any operation and “copy” it.   You can go to your other cut’s setup, and “paste” it.  Works, but clunky.
  • Better, is to select one or more operations in the browser, and RMB on them -> Store as template : This will give you a broswer to your local HD for storage, and later import via the “Create from Template” Setup RMB menu.

Simulate / preview the cut

This is an incredibly powerful part of F360:  You can pre-visualize your cut.  Either select your setup folder in the Browser, or multi-select all the operations you want to preview (basically, whatever toolpaths are shown will be simulated), and press the  ACTIONS -> Simulate button.

In the SIMULATE popup, check on the “Stock” box.  This will show you the uncut stock.  You can uncheck the “Toolpath” if you don’t want the lines to obscure the view.  Then simply press the > Play button at the bottom of the screen:  All the selected operations will begin previewing their cut:

cutPreview

Green is the roughcut, blue is the final pass.

Installing the correct postprocessor

For F360 to generate the correct gcode/nc data, it needs to be post-processed for your given machine.  Since I’m using an Inventables X-Carve (grbl-based), I had to do some searching.  Here’s two links to postprocessors for the X-Carve:

In either case, you can save the .cps file(s) to your local drive rather than uploading them to the cloud like described, they’ll be used in the next section.  Move the data here:

C:\Users\<USERNAME>\AppData\Roaming\Autodesk\Fusion 360 CAM\Posts

Generate or “post” the gcode/nc data

Once you’re happy with your toolpaths and have downloaded a postprocessor, you can ‘post’ the data for your CNC to use.

The big decision here is how you’ll save the operations you’ve made previous:  If they all share the same bit, you can select them all at once in the Browser, and save a single file for all of them.  However, if toolchange is needed, you should save each operation as a separate file, selecting one at a time and going through the below steps.

Via the ACTIONS -> Post Process Menu:

  • Setup : Use Personal Posts
  • This will direct the Configuration Folder to the one you saved the .cps data in above.
  • In the Post Configuration section, select the appropriate .cps file.
  • Define the Output folder where you want the .nc data saved.
  • Under Program Settings, set the name of the file under “Program name or number”.
  • Press the “Post” button:  The .nc data is saved to disk.

Cutting with the data

There are number of sender software available to send the .nc data to your machine:  Easel (browser-based) can do it, I’ve had success with Chlipeppr (browser-based), I hear good things about LaserWeb/CNCWeb (browser-based, not yet tried), but currently use Universal GCode Sender (Java applet)  for all my work.

The F360 data didn’t cut any differntly in UGS than MeshCAM data, and had great result:

finalCut

In fact, the few hard-edges around the hemisphere are due to a pencil-cut I was toying around with as an extra pass.

In Conclusion

I feel F360 provides a tremendous amount of power to the hobbyist CNC user, especially considering the price (free).  The learning curve is a bit steep, but it has a large amount of helpful documentation, and videos available.  It’ll be my go-to piece of CAM software in the future, hands down.

 

New CNC Cut : HexBeam

Continuing to play more with MASH in Autodesk Maya, I came up with this experiment:  I used a ramp node with a wave to mask where the hexagons are placed, then randomized their scale.  Applied a dark stain on the uncut top, and a natural stain on all the hexagons.  Material is a reclaimed redwood beam.

hexbeam

About half an hour of modeling in Maya, and 1h45min on the X-Carve CNC with a 1/8″ 1-flute upcut endmill.  Probably another half hour of sanding.

New CNC cut: Honeywood

I’ve been teaching myself the MASH toolkit in Autodesk Maya.  It’s been a lot of fun to learn.  As a challenge, I decided to design a hexagonal-based structure, which I then cut into some reclaimed redwood with my X-Carve CNC:

honeywood_mash2

I applied a ‘natural’ stain to the inside section, and a darker ‘walnut’ stain to the outside.  The rough cut was with a 1/8″ 1-flute upcut endmill, and I did a pencil-cleanup pass with a 1/16″ 2-flute upcut endmill.  Whole cut took maybe 45 minutes.  The piece measures 8″ square, and the cut is around 1″ deep at the lowest point.  I used MeshCAM to generate the toolpaths from the stl file exported from Maya.

Building the C-Bot 3d Printer : Part 36 : Adding an inductive z-probe to RepRap Firmware / RADDS

Jump to C-Bot blog index to see all the posts.


Introduction

This post describes how I installed an inductive Z-probe on my C-Bot 3d printer, using RADDS hardware with RepRap Fimrware.

My C-Bot printer has a 12″ square build plate, with 4-point screw leveling: Not the easiest thing to keep level.  I decided to tackle installing an inductive Z-probe to help with the leveling, since RepRap Firmware supports it.

Very important:  Before you get started, you’ll either need an aluminum build plate, or some copper tape you can stick on your existing surface at the points you want to probe.

Other info:

  • This sensor works in conjunction with your Z-endstop:  You still home using the endstop.  But after the home, the probe takes over fine-tuning the leveling process.

Get the probe:

I picked up a LJ12A3-4-Z/BY inductive probe off E-bay some time back.  It’s stats:

  • 4mm sensing distance (to iron)
  • NO, PNP
  • 6-36v input, 300ma
  • Brown = Positive, Blue = Negative, Black = signal

Make a bracket:

I modeled up a bracket for it in Autodesk Maya, that would hang off the rear of my hotend gantry.

After the probe was mounted to the bracket, I adjusted the probe so it was about 1mm from the build-plate, if the nozzle was touching the plate.  Basically, a different in 1mm from nozzle to probe-base.

probebracket_web

You can download the bracket from Thingiverse here.

Wire it up:

Voltage Divider:

Update:  I’ve been told you can drive these sensor directly off 5v:  I’ve not tested this,but if you’re going to attempt it, it’s worth a shot.  Save you from having to deal with the voltage divider below, and it means you can wire + & – directly into the RADDS board itself.

The probe needs 6-36v, the signal input on the RADDS board only accepts 5v, and my PSU is 12v:  Need to make a voltage divider!  Generally speaking, you need two resistors, with the smaller one half the value of the larger one. Like 10k & 5k.  Of course none of my resistors worked this well, and even when I did find some that may ‘sort of match’, they value they split wasn’t 5v.

After MUCH combinations, I came up with this:  Big 2k (really 1970 on my meter).  Small was two in a series: 1k (really 970) and 670 (really 660) for a total of 1730:  1730 isn’t remotely half of 1970, not even close.  However when setup on my beadboard, it was splitting out to 5.6v, which was the closest I got all day.

Later I read that anything over 3v would trigger things fine, so I was probably making this way harder on myself than I should have.

Mockup on the breadboard, using my Macbook Air as the ‘inductive aluminum surface’ 😉

breadboard_web

Final shrink-wrapped setup.  Resistors hidden beneath the wrap.

voltage_divider_web

RADDS Board:

The signal line needs to run into the “Servo PWM3 pin” (aka Due digital 39, AKA E0_AXIS endstop[3]), which is located in a cluster of solder-points on the corner of the board:  I soldered in a header, so that I could plug my signal line into it.

radds_web

Connect the wires:

Signal from probe (since having it’s voltage lowered above) -> ‘Servo PMW3’ 5v pin on RADDS board (image above).

Positive & Negative probe leads -> PSU 12v +- terminals.

Update the Firmware:

G32 is the command that triggers the probing on the board.  But the probing can be setup two different ways:

  • Use a bed.g macro filled with M30 commands (and others).
  • Use config.g filled with M557 commands, no bed.g.

I like the idea of having a separate macro file to configure my probing:  If bed.g exists, when you execute a G32, the bed.g is parsed.  If there is no bed.g, G32 instead looks for pre-configured M557’s, that live in config.g.

Initial setup

Below, I discuss how I setup config.g and bed.g

config.g

When you first add the code for the probing in config.g, it’s important that you set the ‘Z offset’ in G31 to 0: You’ll later calibrate it and edit it with the final setting.  Here’s my probing section:

M558 P4 X0 Y0 Z1 ; M558 must come before G31.
G31 X49 Y52 Z.4 P500

To break it down:

  • M558 – Set Z Probe Type
    • P4 : Set the sensor type.  When using an inductive sensor plugged in to the PMW3 pin, you need to set this to 4.
    • X0 Y0 Z1 : Use the sensor for the Z axis only.
  • G31 – Set Current Probe
    • X49 Y52 : This is the distance in mm that the sensor is away from the nozzle (used my calipers to roughly figure this out).  Since my sensor is behind and to the right of my nozzle, these are both positive values, since 0,0 is in the front left of the bed.  You can leave these zero, but I’ve read that having them set makes the calibration more accurate.  However, it makes setting up bed.g more complicated (more on that below).
    • Z.4 : This is the difference in height between the sensor and the nozzle.  Set this to zero the first time you set it up, it will be calibrated later.
    • P500 : The ‘trigger value’ : Really only important if using an IR probe, but I read for switches just set this to 500.

bed.g

This is where you define the points to probe/sample.  I’m doing a 5-point probe, but you can use as few as 3.

The only really confusing part is if you’ve entered any probe offsets in config.g’s G31 (above):  They need to be accounted for below, since you’re telling the system where to send the probe.  If the probe has a 50x, 50y offset from the nozzle, and you tell the probe to go to 0,0, it’ll try to run the nozzle outside the bounds of your printer, and much stepper chattering / printer shaking will ensue until you kill the power.

To calculate the below values, this was my process:

  • Home the printer, G28.
  • In my software (Simply3D), manually jog the toolhead around to the 5 points I want to sample  When I get the probe to a sample spot, I note the current X,Y value (which is for the nozzle), and I add the offset values  to it.
  • Make sure the probe is always over the bed!  If you position the probe off-bed, when it goes to sample that point, it’ll drive the bed straight up into your nozzle :(

My bed.g:

M561 
G28
; Probe the bed and do 5-factor auto calibration
; These are the same toolhead points, but with the sensor offsets added. Note, to use these points, you must set config.g's G31 X49 Y52
G30 P0 X49 Y52 Z-99999 ; Four... - Front Left
G30 P1 X49 Y305 Z-99999 ; ...probe points... - Back Left
G30 P2 X299 Y305 Z-99999 ; ...for bed... - Back Right
G30 P3 X299 Y52 Z-99999 ; ...levelling - Front Right
G30 P4 X149 Y152 Z-99999 S5 ; 5th probe point + store the levelling - Center
G1 X0 Y0 ; Send X & Y back to zero before print starts. This is commented out during the initial calibration.

To break it down:

  • M561 – Set Identity Transform : Clear out any previous probing transformation done.
  • G28 –  Home : Must always home before probing.
  • G30 – Single Z Probe :
    • P# : Each sample point must be assigned an index, from 0-4.
    • X# Y# : the location on the bed to send the probe.  These include the offset set in config.g’s G31.
    • Z -99999 : A value less than -9999 tells the system to probe here.
    • S5 : The final probe has the S value entered, telling it to store all 5 points.
  • G1 X0 Y0 : Send the toolhead back to X0 Y0 before print starts.  Just something I like to do, since I purge the nozzle there.  Note, during the initial calibration stage this is commented out, which makes setting the probe to nozzle z-height easier (more below).

Calibrate the nozzle-to-probe height

As discussed above, I set my proximity sensor to be about 1mm above my nozzle height.  These sensors have a 4mm detection distance for highly inductive materials like iron, but for aluminum, it’s much closer, around 1mm it seems.

Once the config.g and bed.g have been updated, fire up the printer, heat up the nozzle and bed (if you can) and execute a G32:  This will both home, and then start the probing sequence (based on what you’ve defined in bed.g).  Be excited as you watch your printer automatically drive around probing for points!  It’s important the nozzle/bed is heated up, because thermal expansion.

When the probing is done (and everything is still hot), use this process to determine the nozzle-to-probe height difference:

  • You can either enter the below commands, or use some other control software (Simplify3D) to do it.
  • G1 Z0 ;  Send the bed\nozzle to the current Z0 position.  This should move the plate close to the nozzle, but not touch it: Should be 1mm or less away.
  • G92 Z10 ; This tricks the machine so it thinks the toolhead is actually 10mm above the bed.
  • Slip a piece of paper between the nozzle and build plate.
  • G91 ; Set Relative moves.
  • G1 Z-.1 ; Start raising the bed\lowering the nozzle by -.1mm values.
  • Track how many moves you make.  Keep raising the bed\lowering the nozzle until the paper just barely moves:  You should still be able to slip the paper under the nozzle.
  • Write that number down.  Mine was -.4mm.
  • Let your machine cool, power it down.

Update config.g and bed.g

Take the positive value of that number from above, and update your config.g’s G31 Z# with it:  This is now your calibrated offset!

G31 X49 Y52 Z.4 P500

In your bed.g, enable the last line to send the toolhead back to G1 X0 Y0 if you want.

The next time you run a G32 and then send the nozzle to Z0, it should be just touching the build plate, allowing you to slip a piece of paper under it with the same friction as above.  If not, something is amiss.

However, it’s possible this position still isn’t optimal for printing the first layer:  I did a test print with a hollow cube (no roof, no floor, 2 shells) just slightly smaller than my build volume.  The nozzle was still slightly too high for good first layer adhesion.  Rather than constantly updating your firmware value to try and tweak this, you can use your slicer software, covered below.

Update your print Profiles:

My slicer software is Simply3D, but I’m guessing other slicers (Slic3r, Cura, etc) work similarly.

Start Script

The start script is the gcode that is execute before a print starts.  The only change I had to make was switch out the line that did the home operation (G28) with the new G3d command, which calls to bed.g, which homes and probes.  This is what mine looks like:

G92 Z0 E0 ; Set current z position to zero.
G1 Z2 ; Lower Z to be safe 2mm.
G32 ; bed.g - home and probe bed - If not probing, this would be G28 instead to just home.
G1 E50 F600 ; Purge nozzle 50mm 10mm sec When a print ends it's retracted by 30mm.
G92 E0 ; zero extruder
G1 X0 Y10 ; Move nozzle to left front corner of build platform.
G92 X0 Y0 ; Zero X & Y here to start the build.

Refine the Z-height

As mentioned above, my first layer was a bit too high, and wasn’t quite sticking right.  Simplify3D has a section in its ‘G-Code’ menu called ‘Global G-Code Offsets’: These allow you to provide an additional global offset to all values in the gcode.  As it turns out, setting XYZ to 0,0,-.025 mm made for a great first layer.  Iterating with this value is far easier/faster than updating the firmware.

Thoughts for dialing this in:

  • With the Z value set to zero (the default), do a test print of a box with a solid bottom.
  • If the first layer doesn’t stick well enough, cancel the print, lower by -.02 and try again.  If you see the extrusion curling up and off the bed as it extrudes, it’s actually to close, and add .02 and try again.
  • Keep iterating on this process until you get a nice stuck first layer.

Final Thoughts

Now that it’s working, I’m so sad I did’t do this sooner.  Full-volume first layers are just ‘spot on’ now.  It’s almost magical to watch it work.  Get an aluminum plate and do this mod!

Resource List:


Jump to C-Bot blog index to see all the posts.

New 3D Print: Millennium Falcon

Decided to print (nearly) a whole roll of MakerGeeks Gray Matter Gray PLA on a cool Millennium Falcon model I found on Thingiverse.

Took 17h30m on my C-Bot, using a .6mm E3d-v6 Volcano nozzle, 450 micron, 60mm\sec @ 230 deg:

falcon

It’s pretty big.  Check out the timelapse here:  17 hours in 17 seconds: