Cut2D is 2D CAM program from Vectric. It is designed to quickly and easily import DXF plus several other vector formats and create G Code for CNC cutting. It is primarily designed for traditional mills and routers. While I would not recommend purchasing it to only use on a laser, people who have both a CNC router and a DIY laser will find this to be a very capable and inexpensive product.
I have used Vectric products for years. I started with VCarve, then upgraded to Aspire. A forum member recently asked for help using Cut2D. Vectric was gracious enough to give me free evaluation copy. This is probably due to the fact that I already own their top of the line product. They did say that they are not really interested in selling it for laser use only because the program may be confusing to them and they only want 100% satisfied customers.
The Vectric products ship with 100+ pre-made post processors. There are several flavors of Mach3 post processors that will work right out of the box for most mills and routers. It is also very easy to customize your own post processor. I created one for Aspire last year and found that it worked perfectly for Cut2D as well. I wrote a blog post about it and the file is available here. All Z movement is removed from the post processor, so the actual Z values used below are not going to affect your machine while cutting.
I am not going to explain how to use Cut2d. Vectric does a great job of that. I will just explain the differences when using a laser cutter.
Creating a Laser Tool
The first step is to setup a “tool” in the tool library for the laser beam. The beam can be thought of as an end mill. It is basically a cutting cylinder with a fixed width. The major difference is that it has an “infinite” depth of cut. In reality most lasers are not going to cut anything thicker than an inch or so due to beam divergence.
Many values you set are just default values and can be changed when you use the tool for a cut.
Tool Name
I called my tool “Laser Beam 0.003″. If you want to go crazy, you could setup dozens of tools with default values that work well with certain materials. You could name the tools “1/8 Plywood laser cut” or “6mm Acrylic laser cut”, for example. This way you do not need to remember what speeds and feeds are needed for each material.
Tool Diameter
Cut2D will use this when calculating how much to offset the cut line from the geometry when cutting inside or outside features. An easy way to determine this is to cut out a 1 inch square on the geometry lines with no offsets. Measure the actual size of the part. The amount you are less than the inch will give you the beam diameter. If you want to be as accurate as possible, you could define multiple tools based on different materials and thicknesses.
Pass Depth.
You cannot realistically use Cut2D to control the depth of a laser cut. Therefore, this value is not important. You do want to make sure this value is larger than any value that you will use when specifying tool paths so the cut is always one pass. I suggest setting this to a value of 1 inch. This default value can always be changed when you are setting up a toolpath if you actually want to play games with multiple passes.
Stepover
This does not apply for lasers, because we will not be doing pocketing. Just set it for 45% to keep Cut2D happy.
Spindle Speed
This value is also not really important at this point. You could use it to control beam power if your laser supports that. If your laser can use this for beam power then set it for the number that would yield max power, otherwise a value of 1000 should be fine.
Feed Rate
Again, this is a default number that can be changed at each tool path, so pick number that is close to t typical number you might use.
Plunge Rate
This does not apply so just put in any reasonable value.
Here is what a typical laser might look like.
Usage
I will explain one cut using the wing_spar example file that comes with Cut2D. The cut will be the inside features of the wing spar.
Select all the inside features and then click the Create Profile Toolpath icon on the toolpaths flyout menu on the right.
Cutting Depths.
These values do not matter. You just want to make sure the cut depth is less than the pass depth set for the tool. This will insure that only one pass is done. Advanced user could of course use this to setup multiple passes.
Tool
This is where you select your laser tool. Use the edit button to set the actual cutting speed you want.
Machine Vectors.
Use this to tell Cut2D what side you want the tool offset to. The direction setting (climb or conventional) is primarily for spinning tools, like end mills, but if you care which way the cut goes around the loop, you can change this.
Ramp moves
Don’t use this.
Tabs.
Tabs are primarily used to keep parts in place with spinnig tools, but you might want to take advantage of it to keep light parts from blowing around, or if you want all the parts to stay on the material after cutting.
Outputting the G Code file.
The last step is to output the file using the custom laser post processor. A copy of the file is available here.
Good luck. You might want to try a few dry runs with the laser disabled and you hand on the e stop button to make sure it works for you.