RWO (Rotated Work Offsets) Tutorial

Similar to Haas' Dynamic Work Offsets (DWO) and Fanuc’s Tilted Work Plane Indexing modes, Pocket NC’s Rotated Work Offsets feature allows users to set a work coordinate system (WCS) origin that is relative to a point on a part or its stock, instead of a point that is relative to the machine (typically the center of rotation). This allows the stock to be loaded onto the machine differently than it is modeled in the CAM workspace while maintaining the ability to perform positional 5 axis tool paths, otherwise known as 3+2 machining. Below are the basic steps to follow when programming and running a part using RWO.

This tutorial uses Fusion 360 as the CAM software to generate the tool paths and g-code but the same concepts should apply to any other CAM software that has a post processor that supports RWO on the Pocket NC V2 machines.

Step 1: CAM Setup

After it has been decided that a part will be programmed with the intention of using RWO, the first step is to configure the CAM setup accordingly.

• Begin by creating a new setup.

Open

• Next, orient the part the way it will sit on the machine when the A and B axes are at 0 degrees. Then use “Select Z axis/plane & X axis” to orient the WCS the way the machine’s axes are oriented when looking at the machine from the front.

Open

• Now pick your preferred origin point for the WCS. It is usually best to pick a point on the stock that will be reachable with a tool or edge finder before any machining has been done. Below, the corner of the stock that is closest to the spindle and the front of the machine has been chosen for ease of access.

• Next, move to the “Stock” tab (yellow cube at the top of the setup window) and begin defining your stock and its position relative to the part. The example below shows a 2” cube that is centered around the part in the X and Z directions and just .010” higher than the part in the Y positive direction.

• Lastly, move to the “Post Process” Tab. Here you need to give your program a name and comment as well as pick what WCS offset you want to use. In this example, we are using WCS offset 1 because we want to use the G54 code to define our work offsets on the machine. You may use any number from 1 to 8 here, just make sure you are aware of what G5x the number corresponds to.

Step 2: Tool Path Application

Now that the setup is configured correctly, tool paths can be applied. Tool paths and machining operations can be configured using the same method used when programming around center of rotation. The only difference will be where the WCS is displayed relative to the model, but as long as it is oriented the way it needs to be to cut the desired feature, there will be no effect on the final tool path. For more information on applying tool paths in Fusion 360, check out the V2 Series First Part Tutorial.

Step 3: Post Processing

With all of the tool paths created and the part ready to cut, it is time to post process the tool paths into g-code.

• Begin by right clicking on the setup that was created in step one, in this example we have named it “Setup 1”, and then select “Post Process”.

• Next, adjust your post processor window to the settings shown below, ignore the “Properties” for now. (Mac and Windows computers have different post processor windows so both are shown). The program number and program comment can be whatever you would like.

• Now, in the Properties section, locate the property titled “Rotated Work Offsets WCS” and click on the word “Disabled” next to it. This will create a drop down menu, giving you the option to choose what WCS you would like to use to store the rotated offset values. It is important that you do not choose a WCS that is already being used by your program (found in the Post Processor tab of of your program’s setup). WCS number 9 (G59.3) should be fine to choose here if you followed the instructions in Step 1 exactly.

• Next, locate the property titled “Machine Model” and select the model of Pocket NC machine that this program will be run on.

• Finally, post process the g-code by clicking “OK” or “Post”. You will be prompted to choose a location to save the g-code to as well as name the file. It is good practice to keep the .ngc file extension on the file name. The g-code will then be displayed in your computer’s default text editor or something similar (seen below for Mac and Windows).

Step 4: Machine Set Up

After g-code generation, the machine has to be set up. The majority of this process is the same as setting the machine up to cut a part that is programmed around the center of rotation:

• Turn on the machine and home its axes.

• Install necessary fixtures.

• Install and measure the tools that will be used. For V2-50 machines simply install and measure the first tool that will be used, the rest will be measured automatically at each tool change.

• Install the stock material, locating it on the fixture in the orientation that was planned at the start of the CAM programming.

Step 5: Setting Work Offsets

This step is where the machine is told what point all of the g-code coordinates originate from. There are several ways to perform this process but in this example we are going to use the simple touch-off/paper method.

• Begin by installing the tool (usually an endmill) you wish to use for this process. Tools with 3 or more flutes usually work best. You may also use the shank of a tool or a precision dowel pin. In this example, we are using an 1/8” single-flute endmill that has been turned around in the tool holder.

• Now, measure the tool that was just installed. If the tool being used to set work offsets is not a tool that will be used in the program (which was already measured in Step 4), you will need to pick a tool number that is not being used and measure the tool using that line of the tool table. In this example we are using tool number 15.

Setting Z Work Offset

• Begin by using the jogging controls in the Pocket NC user interface to position the touch-off tool to the right side of the stock, inside the front face and below the top of the stock.

• Next, the machine needs to know how long the tool is so that the DRO readout is accurate. To do that, call up the TLO (found when the tool was measured) by typing “G54 G43 H15” into the MDI command bar and pressing enter on the keyboard. A green check mark will appear in the MDI bar when the command has been activated.

• Then, using .01” steps, jog the tool towards the stock in the Z negative direction. Be careful not to go too far and collide the tool with the stock. Once the tool is as close to the stock as it can be using .01” steps, insert and hold a thin piece of paper between the tool and the stock. Now switch to .001” steps and continue to move the tool in the Z negative direction until the paper has been pinched.

• Lastly, set the Z work offset by navigating to the “Work Offsets” section of the Pocket NC user interface and clicking on the input box in the Z row and G54 column. A drop-down menu will come up allowing you to choose “Zero DRO”.

Setting the X Work Offset

• Begin by using the jogging controls in the Pocket NC user interface to position the touch-off tool in front of the stock and just below the top of the stock.

• Then, using .01” steps, jog the tool towards the stock in the X positive direction. Be careful not to go too far and collide the tool with the stock. Once the tool is as close to the stock as it can be using .01” steps, insert and hold a thin piece of paper between the tool and the stock. Now switch to .001” steps and continue to move the tool in the X positive direction until the paper has been pinched.

• Lastly, set the X work offset by navigating to the “Work Offsets” section of the Pocket NC user interface and clicking on the input box in the X row and G54 column. A drop-down menu will come up allowing you to choose “Set DRO to a Value” and then you will be prompted for the value. The value used in this example will be -.0625 because that is the radius of the tool we are using, which means that is how far the center of the tool is offset from the face of the stock in the negative direction.

Setting Y Work Offset

• Begin by using the jogging controls in the Pocket NC user interface to position the touch-off tool on top of the stock near the front corner of the stock.

• Then, using .01” steps, jog the tool towards the stock in the Y negative direction. Be careful not to go too far and collide the tool with the stock. Once the tool is as close to the stock as it can be using .01” steps, insert and hold a thin piece of paper between the tool and the stock. Now switch to .001” steps and continue to move the tool in the Y negative direction until the paper has been pinched.

• Lastly, set the Y work offset by navigating to the “Work Offsets” section of the Pocket NC user interface and clicking on the input box in the Y row and G54 column. A drop-down menu will come up allowing you to choose “Set DRO to a Value” and then you will be prompted to for the value. The value used in this example will be .0625 because that is the radius of the tool we are using, which means that is how far the center of the tool is offset from the face of the stock in positive direction.

Step 6: Simulate and Run

After setting the X, Y and Z work offsets, your machine should be ready to run. You can simulate your program in the newly updated Pocket NC Simulator by uploading the g-code, pressing the stop button and then inputting your TLO and work offset values in the summary tab. More details on how to use the Pocket NC Simulator can be found in this video.

Using RWO can add another place to make a mistake when setting up the machine so when you are ready to run the program it is always a good idea to watch the part run all the way through to make sure that everything runs like you expect.

If you have any questions about using RWO, please feel free to reach out to us as service@pocketnc.com.