CNC West Oct Nov Web

56 CNC WEST October/November 2018 CAD/CAM/CNC Perspective By: Tim Paul Manager- Manufacturing and Business Strategy Instagram: OneEarTim To comp or not to comp... types later. M ost CAM systems offer different compensa- tion types. See Figure 2 for the list Fusion 360 offers. “In computer”, “In control”, “Wear”, “Inverse wear” and “Off” are the common compensation types. “In computer” and “Wear” are the most com- mon compensation types I see being used in indus- try. Here is a basic run down of the different types and why I would use them. I n computer - The toolpath is offset from the feature geometry by the radius of the selected tool in the CAM software. I mostly use this when roughing, or when machining features I don’t plan to adjust the size. Examples: When roughing I may have a .010” stock to leave allowance, but my tool size typically only varies less than .001”. So, there is no need for tool compensation. Also, roughing cycles don’t typically offer tool compensation options. When no compensation type is offered the default is “In com- puter as the CAM system will offset the toolpath by the radius of the selected tool. I also use “In comput- er” when chamfering because I buy quality tools that have accurately defined tip diameters, I use consis- tently accurate tool offset measuring and rarely need to adjust my chamfer size. I n control - The toolpath centerline is output to fol- low the feature geometry. The output code includes a G41 (right comp), or a G42 (left comp) to offset the tool by the tool radius pulled from the diameter offset table in the machine control. Offset table example: A ¼” tool should have .250 listed in the diameter offset table in the machine control. The output code also includes a G40 to cancel the compensation when the tool path is complete. “In control” is an older method of cutter comp. As I mentioned earlier I and many others used this type of cutter comp when pro- gramming parts by manually writing G-Code. This A few days ago, I was at a friend’s shop. He is someone I would consider a competent machinist, pro- grammer and business person. Most of his business involves rapid prototyping parts for Silicon Valley and Bay Area companies. Many of the parts are complex. After a part was done, I watched him measure a bore, do some math and then run back into his office and made some adjustments to his program. He reposted the program and re-ran the bore operations. I was a bit surprised and asked what he did. He explained that he needed to bore another .0015 larger, so he went into Fusion and changed the stock to leave to a negative to adjust the size. I always say that whatever process you have that makes good parts and is profitable is an acceptable process. But, I’ve since found out that there are a lot of people not using cutter compensation to adjust the size of their features. So, I thought it was time to write something about it. W hat is cutter compensation? Cutter compen- sation (Cutter Comp) as most people use it can also be called Cutter Diameter Compensation (CDC). Cutter Comp provides a way for the tool path to be adjusted at the machine to compensate for tool size, tool wear and tool deflection. When I originally started programming by manually writing G-Code I utilized Cutter Comp to offset the tool by Figure 1 the radius. This allowed me to program tool paths centered along the part features rather than having to offset the tool path geometry to compensate for the tool size. Figure 1 shows how CDC Right (G41) causes the tool to move to the right of the pro- grammed path to adjust the feature size. N ote: Cutter comp must be turned on or off with a line move, never an arc. Commanding G40/G41/ G42 with an arc move will cause a diameter com- pensation error that will stop the program. Notice the line move labeled “Lead In Line” in Figure 1 as cutter comp is activated. The line move needs to be longer than the radius of the tool in the diameter offset table of your machine control. Remember this as I talk about “In control” and “Wear” compensation