Introduction: Generating Gcode for ShopBot From AutoCAD File Using Vectric Cut 2D

Going from an AutoCAD file to gcode sounds complicated, But today's software makes it relatively easy.  This Instructable will show you how to take an AutoCAD file, export it as a .DXF file, import it into a software package called Vectric Cut2D, and then create a gcode file for use on a ShopBot. 

I am a member at a DIY workshop called TechShop.  They have the AutoCAD and the Vectric software I am using available for all members to use. They also have CNC machines such as the ShopBot, that I will use to actually cut the holes in this faceplate (in another Instructable yet to be done)..

The project used in the Instructable is to be the front panel of a homemade DC power supply.

First you open AutoCAD and your file.  Then save it as a .DXF.  To do this, click the main pull down at the very top left letter "A" and select "Save As".  From the window that pops up select "Other Formats."   In the standard windows save dialog box, go to file type drop down menu and select "AutoCAD 2004 DXF".  Saving in later versions of AutoCAD does not work with the version of Vectric Cut2D that I have (don't know why).

Step 1:

Open Cut 2D.

Step 2:

Click "File", "Import" and then browse and find your .DXF file.  This is the resulting window.  You can see the file has been imported and a settings dialog box pops up.

Step 3:

In the dialog box, all I need to do is set the thickness of my material, which happens to be .125 inch. All other settings are correct.  Click OK.

Step 4:

What we are left with in the part window includes text I am not going to be cutting so I want to delete the text.  (This is not required but I think it makes it simpler to see what you are doing).

Step 5:

Delete the text by using your mouse to draw a window around it and then simply hit the delete key.  The screen capture shows that all but the "POWER" text has already been deleted.  When you select it with your mouse, it changes color.  When done with deleting any text, go to the next step.

Step 6:

To create a cut path, Cut 2D requires that all lines in the drawing be reliably connected/joined together. I happen to know the 4 lines in the rectangle are joined at the corners already so will do nothing there. But the lines in the 12 oval like holes are not (a quirk of how I drew them in AutoCAD - yours may all be connected properly).  So, using your mouse, draw a window across all of the oval shaped holes and select them all. Then hit the join vector button - go to the left panel and locate the first button above the words "Align Vectors".   It will be an oval with 5 yellow dots. Click this button.

Step 7:

The following dialog box will open - you can see from the dialog that there are many lines that are not connected.  Click "Join" and the task will be done.  Then simply click "Close".  Our model is now ready for tool path design.

Step 8:

Click the "Toolpaths" tab in the upper right and a window will slide out.  In the field of icons, click the 2nd from the left in the top row.  This will allow you to cut what is called a profile (translation - the CNC mill will just cut an outline of the rectangle and holes I need cut).

Step 9:

This dialog box comes up.  You must set the depth you wish to cut to (I set it at .130 inch).

I want the cutting tool to cut inside the line of my geometry as that is the exact size I want, so I click"Inside".

I did nothing with the plunge or tab area (some will rightly argue I should do tabs - this puts a small tab in the cut file that holds all the pieces being cut on the table - it prevents any opportunity of them flying off after cutting, but you then must cut and file the tabs away).

Step 10:

Now click the "Select" button under "Tool".  A dialog box will appear that allows you to set a variety of settings.

1.  I picked a .125" end mill.  
2.  I set the cut depth per pass at .026 inches (5 passes to get through to .130 inch depth I set earlier)
3.  I set the feed rate at 20 inches per minute (this is how fast the end mill moves sideways when cutting)
4.  I set the plunge rate at 10 inches per minute (this is how fast the end mill descends into the material)
5.  I set the RPM to 15,000.

Step 11:

Next, use your mouse to select all the figures left (rectangle and all of the oval like figures).

Then hit "Calculate".

Step 12:

This dialog comes up because I am cutting to a depth (.130") that is thicker than my material (.125") and I could be ruining the bed of the CNC Mill I am going to use.  In my case, I have sacrificial material underneath my part being cut so it is OK that it goes through the material.  I click OK.

Step 13:

What then shows up is a visual representation of the tool path.  

Step 14:

Since I want to see the actual cuts, I again go to the Tool, click on "Reset Preview" and "Prepare All Toolpaths".

Step 15:

I end up with a preview of the cuts that shows I have programmed it properly.

Step 16:

Finally, I click on the "Toolpaths" tab again and go down and click the "Save" icon (looks like a floppy disk in blue, 2nd row, furthest to the right).

Step 17:

A new dialog box pops up. I make sure the profiles I want cut are selected in the upper box, and use the drop down menu below "Post Processor" to pick the machine I am going to be using.  It is not shown but there are a huge number of machines in this drop down list - in my case I am using a ShopBot, using inches.  I click "Save", name my file and I now have a gcode file, with the file extension .sbp that I can put on a USB memory stick and take to the ShopBot to cut the holes in my faceplate!