DXF FILE IMPORT CONFIGURATION

Using DXF files is probably most common way to start with machining your first CAD design with your CNC machine.
This short tutorial is made to show you how to configure your imported DXF file in different scenarios. Here are some short examples
on how to configure your DXF files for different scenarios, so that you can get satisfying results on your machine as soon as possible.
We start by clicking File/Import/DXF.

Import user dialog will apear:

Since DXF files have no embedded units, you must define measurement units. Millimeters or inches can be specified.

If you click Advanced, you will be able to set parameters in all three tabs: General, Safe Height and Stages:

General Tab

Use layers

Elements within DXF files are usually grouped in layers. If you choose to use them, you will be able to see certain layers name
in generated G-code window. Use layers feature also allows you to generate Pause and make Tool Change procedure in-between layers.

If your elements are given default layer names, you are able to see these layer names in G-code window. Specific layers name will
appear in the beginning of layers corresponded G-code. This way you can make your generated G-code slightly more transparent.

From picture above, you can clearly see where each layers corresponded G-code begins with execution.

Use pause

Pause will occur at the beginning of specified layers G-code. User dialog will remind you that ‘Pause’ has been generated
and to resume program you must click Continue button.

Tool change

If you want to change tools between elements during your machine job, you can use tool change feature.
Tool change will occur at the beginning of specified layers G-code.

Note: Tool change must take place at its designated coordinates. Tool Change coordinates can be set among
other parameters referring to Tool Change in: File/Settings/Tool Change

Tab

If your work piece doesn’t need to be cut-ed out completely and , you can use tabs to hold the piece in place.
Define length of tab with Tab Size and the distance between two tabs with Tab Distance.

You can see that Tab Size is the un-milled part of toolpath and Tab Distance is where milling will be applied.

Passes and Step Down

With Passes and Step Down you are able to define number of passes that machine will do over generated toolpath
at defined depth increment of plunge per pass.

If surface of your working piece is set to be current Z offset, then value of Base Height will be the depth of machines first plunge move.
This is set in Safe Height tab under Base Height.

E.g.: If you want to cut material of thickness 10mm, and you want to cut it in 5 passes, you could set:

Passes: 5 and Step down: 2.000. What will happen is this: Machine will cut over generated toolpath in 5 passes total.
For each pass machine will plunge for 2mm.

Output control

Outputs ‘Spindle’, ‘Mist’ and ‘Flood’ can be turned ON and OFF in specified moments of tool-path milling process.
How outputs will be controlled depends on what type of cutting will be applied, what materials will be used etc.
Therefore you can set at which point in the milling process outputs would be turned ON/OFF using DXF import dialog.

You can set output ON/OFF control in different tabs of DXF import dialog. It can done in General tab, Safe Height tab or Stages tab.

General tab

If outputs need to be turned ON at the beginning of milling process and turned OFF at the end of milling process, enable ‘Spindle’, ‘Flood’ or ‘Mist’ checkbox in General tab.

Specified outputs ‘ON’ G-code ‘M03’ will be generated at the beginning of toolpath, and specified output ‘OFF’ G-code ‘M05’ will be generated at the end of toolpath.

 

Safe Height Tab

If traverse moves of your machine need to be at certain height, you enable and define this in Safe Height tab.

Enabled output will be turned ON at Safe Height before downward plunge move, and turned OFF at ‘Safe Height’ after downward plunge.

Stages Tab

If you need to turn outputs ON at certain heights you can use Stages feature. This comes very useful if you will be using plasma CNC cutting machine.
When stages are enabled, certain elements machining is divided in stages. Height of stage is where desired output will be turned ON.

 

Stage configuration from picture above will result on CNC machine as:

Elements machining will be divided in two stages. If you have Safe height enabled and set (this is done in Safe height tab),then machine will make downward plunge move
from safe height,it will turn ON ‘Spindle’ output at height 3, wait for 5 seconds (Delay of stage 1)and continue with downward plunge move.
At -1 height, ‘Flood’ output will be turned ‘ON’, machine will wait for another 2 seconds (Delay of stage 2) and continue with the rest of elements toolpath. When milling
of toolpath is finished, both outputs will be turned ‘OFF’ at safe height.

Generated G-code for current Stage setup looks like this:

 

USING MDI IN CNC USB CONTROLLER SOFTWARE

MDI stands for ‘Manual Data Input’. MDI window is located in the bottom right corner of CNCUSB controller software main window:

By entering MDI shortcuts or g-code commands in this window, user can quickly access desired feature, executes g-code command or performs machine specific task.

MDI shortcuts:

You probably already noticed that almost every feature in almost any menu has a number written on the right side of its name starting with symbol “/”. This is its unique MDI shortcut.

If you don’t have any idea about MDI and of its use, it would the best to start with typing “/101” in MDI window and see what happens. Now enter “/151” into MDI window.

First MDI shortcut executed ‘Open’ dialog and second one opened ‘Settings’ menu.

You can browse trough files or change settings configuration with less mouse clicks than if you would click your way trough the menus.

From operators point of view this reflects as more fluent and prompt way of working with machine.

Using arrow keys “Up” and “Down”, user can navigate trough history of previously used MDI shortcuts or MDI g-codes.

One of the best advantages of MDI is gained accessibility of many features provided by CNC USB controller software.

Pretty common step when preparing your workpiece for cutting is setting offsets or capturing points. All these features can be accessed or set using MDI.

Setting XY offset:

If you would want to set XY offset at current machines position, you could click: Machine/Offset/Current XY.

You could do the same thing just by entering “/45251” in MDI window:

Capturing Camera Point:

MDI is especially useful for certain repetitive procedures, like capturing points with camera.
If you want to capture point using camera, you could click Machine/Capture & Measure Points /Capture/Capture Camera Point. You would have to do that for every point you would want to capture.

You could do the same just by entering “ /48102” in MDI window:

If you run a feature directly from menu or a toolbar, then from that point on, this feature will be available in MDI history, and you can find and select it with arrow keys.

MDI g-codes:

You can set and perform machine moves, control outputs or change tools directly from MDI window.

Examples:

Machine traverse and feed moves:

Typing [G00 X10] moves machine to X=10 position at traverse rate.

Typing [G00 Y-20] moves machine to Y= -20 position at traverse rate.

Typing [F100 G01 Y10] moves machine to Y=10 position at feed rate = 100.

Output control:

Using M3, M5, M7, M8 and M9 g-codes you can control outputs:

Typing [M3] will turn Spindle ON and [M5] will turn Spindle OFF.
Typing [M7] will turn Mist ON and [M9] will turn Mist OFF.

Tool change:

You can change or select tool directly from MDI window:

Typing [Tn M6] changes tool.
Typing [M61 Qn] selects desired tool.

Configuring machine settings:

Some machine settings are very easy to be configured with the use of MDI. One of them is whether machine operates in ‘Absolute Distance Mode’ or in ‘Incremental Distance Mode’.

G90 – absolute distance mode:

To move machine in ‘Absolute Distance Mode’ on location of [X10, Y10, Z10] you can enter this command:

G91- Incremental distance mode:

To move machine in ‘Incremental Distance Mode’ for distance of [X10 Y10 Z10], you enter this command:

G53 – absolute machine coordinate system:

You can set your machine moves in absolute machine coordinate system.

To move your machine in absolute machine coordinate system on location of [X10, Y10, Z10] you can enter this command:

Wireless keypad or Shuttle PRO are very practical to work with MDI and for operating with CNC USB controller in general.

MDI offers many possibilities for operator and it is best that each user explores the possibilities of the MDI for itself.