Servo - July 2015

make your job much easier. Look for this feature when selecting your drafting software.

Continuing, I add a rectangle inside the one just created. This can be done manually or — as shown in Figure 6 — by using the contour tool. This extra rectangle is where I will mill a pocket into the box top. Stay with me here; you will see the method to my madness in the next stage. The contour tool is one that I use in many of my drafting sessions. This is another feature to look for when selecting your drafting software.

Drafting — Step C

I use the export feature, and export the drawing into a format my CAM software can use. In this case, it is the EPS file “dominobox.eps” shown in Figure 7. I have found that the Encapsulated PostScript works best when transferring drawings from CorelDraw to Vectric CAM software. Your results will vary depending on the actual software you are using. If you get wacky results, go back and try a different format.

This ends the drafting stage of my process. That said, it’s not really the end. I often have to go back to the drafting stage and make tweaks. Think of it more as the “back to the drawing board” stage.

Tool Path Creation

To create tool paths that your CNC can follow, you need to use a CAM package. By the way, CAM stands for “Computer Aided Manufacturing.” The CAM packages I use come from a company called Vectric. For 2D or 2.5D (as it is sometimes called), you can use Cut2D or its big brother, VCarve Pro, or its grand pappy, Aspire. The interface is the same on all of them. They are differentiated by the number of features and the amount of drafting they allow you to do.

While all of them support drafting or CAD to one degree or another, I prefer using my stand-alone CorelDraw CAD software for this. Since that is its main function, it does it very well. For this article, Vcarve Pro is shown, but the Cut2D software is nearly identical — although it does have some size limitations.

Tool Path Creation — Step A

To start, I load the “Domino Box.eps” file into VCarve Pro. The software starts you out in the “Job Setup” form as shown in Figure 8. Here, notice that the software has properly set our stock size. Next, I add the measured thickness of the stock. In this case, it is .3085.

I uncheck the “Use origin offset” and check the “Center data in job” options. For this job, something that is very important is the XY origin position. I set it to the left rear point. This is because I will be zeroing the machine to the rear vise jaw and to the vise stop placed to the left of the vise. Note that other jobs may require other origin settings. It all depends on where you are referencing zero on your machine.