Cart 0

Creating PCB's using the Zmorph VX

Posted by Grant Cameron on

Creating PCB's using the Zmorph VX

This is the first article out of four that will explain you how to create your own PCB board using the Zmorph machine.

The first step is designing an electronic circuit using any CAD software. For example: Eagle, KiCAD, Altium Designer, OrCAD.

Next step is to export your electronic circuit into a file with GERBER format.

Now you have to create gcode files for your machine. This part of the tutorial will be explaining the process.

We recommend using our version of open-source software FlatCam. It can be downloaded from this link: FlatCAM. Right now only Windows version is available.

Full manual for FlatCam software is available on this site: FlatCAM Manual

For this tutorial, we will use already prepared GERBER files. You can download them from this link: Tutorial Files.

After downloading files from both links please open the FlatCam software from the FlatCAM.exe file. Next step is to load a representation of the CNC table that will help you position the PCB design on the table. To do it go to "File" and from drop down menu select "Open Project..." function and open "ZMORPH_VX_CNC_TABLE" file from tutorial files.

After opening the project your FlatCam should look like this:

Now we can upload a GERBER design. Go to "File" and from drop down menu select "Open Gerber..." and choose "test-F.Cu.gtl" file.


Now we can position our board in the middle of the work table. To do it you have to select the design in the list on the left.


Change the tab to "Selected".


Changing the position of the design is performed by setting an offset. This function does not work with absolute coordination system. The selected item will be shifted by the value that was set by the user.

For example, to position the plate in the middle of the table set a value "(75, 75)" and press "Offset" button. After this project should look like this:


Now we can upload and edge of the PCB plate that will be used as a path to cut out the engraved part. Go to "File" and from drop down menu select "Open Gerber..." and choose "test-Edge.Cuts.gm1" file. Again the GERBER file will load in the left bottom corner as a default position. Shift this design also, using the same offset values as before. At the end you should receive this output:


Next step is to set proper values for CNC milling and laser engraving and creating a gcodes for both processes.


Laser Engraving

Firstly we would like to mark non-copper regions. Non-copper region is an area where the copper is supposed to be removed later on.

To create non-copper regions select the design of our PCB "test-F.Cu.gtl". Double click will automatically move us to the "Selected" tab. In "Selected" tab look for "Non-copper regions" option.


Pressing "Generate Geometry" will create new geometry on the list of project elements, the new geometry will be called "test-F.Cu.gtl_noncopper".


Double click on the newly created element to move to "Selected" tab. Now look for "Paint Area" section and edit the values as follow:

Tool dia: 0.12

Overlap: 0.5

Margin: 0.0

Selection: All


After changing the settings we can generate the new geometry by pressing "Generate". This process might take a while. When the process is finished the new geometry called "test-F.Cu.gtl_noncopper_paint" will be created.

Then again double click on newly created geometry to enter "Selected" tab. Now we will focus on "Create CNC Job" section. Set the values as follow:

Cut Z: -0.0024

Travel Z: 0.1

Feed Rate: 1800

Tool dia: 0.12

Spindle Speed: Leave empty

Multi-Depth: Checked

Depth/pass: 0.0004


When all values are set we are ready to press "Generate" to create a gcode for laser engraving. New object will be created and your project should looks like this:

Now by entering the "Selected" tab for "test-F.Cu.gtl_noncopper_paint_cnc" we will have option "Export G-code" available. Use this option to save the gcode. Remember to set the name and add ".gcode" at the end of the name.

Right now we have the gcode ready for laser engraving.


CNC Milling

After engraving the plate with laser next step is to cut out the PCB from laminate.

Double click on "test-Edge.Cuts.gm1" and in newly opened tab "Selected" move to "Board cutout" section.


"Tool dia" is a diameter of the cutter that we are going to use for CNC PRO job.

"Margin" is a offset from the Gerber project cutout lines.

"Gap size" is a size of each bridge automatically created by the software.

"Gaps" define a number of gaps used.

  • "4" will make four bridges in total , one on every side (left/right/top/bottom).
  • "2(T/B)" makes two bridges, one at the top and one at the bottom of the design.
  • "2(L/R)" makes two bridges, one at the top and one at the bottom of the design.

Press "Generate Geometry" and wait for the software to finish the operation.

Now the new geometry will be created, "test-Edge.Cuts.gm1_cutout". From this geometry we will prepare a path for CNC milling. Select the new geometry and go to "Selected" tab. Look for "Create CNC Job" section and set the values as following:

"Cut Z" - Same as a thickness of used material. 

"Travel Z" - Set for 2 as a recommended safe value.

"Feed Rate" - Recommended value for this set up is 60.

"Tool dia" - The same as before so 2.

"Spindle speed" - Leave empty.

"Multi-Depth" - Checked.

"Depth/pass" - 0.5 for "Tool dia" 2

Share this post

← Older Post Newer Post →