Generate the G-code

First task to do is to generate a stereo lithography model using your 3D CAD program that can be imported in Vectric Cut3D with the basic rule that you should only export what needs to be milled. Holes for example need to be drilled, if the hole is part of the model and the diameter is larger than the diameter of the finishing mill than the mill will mill the hole which in many cases does not result in a perfectly round hole. It’s better to hide or suppress these holes before generating the model and before the part is milled drill the holes in the stock at the correct locations.

The model

In the example the largest hole is 5.9mm and the finishing mill will be 6.0mm so no holes need to be removed. Export the model to a STL file, two parameters are important: deviation or chord height and angle control or angle tolerance. Typical values for 0.025mm for deviation or chord height and 0.5 for angle control or 10 for angle tolerance. In Pro Engineer, select 0 for Chord Height, this will trigger Pro Engineer to calculate and set the minimum value. For Angle Control use the value 1.

Open the STL file in Cut3D, click on the options of the radio control that control the top surface. The model in the 3D view will represent how the model will be cut out of the stock and how it will be oriented on the machine table. Make sure the units are set to the same units as you used during the design in your CAD program. Select the 2- Top and Bottom sides to machine and apply the settings before clicking the next button.

Note: Write down the part sizes as Cut3D reports them, they are needed in a later stage during the milling process.

Step 1

First use the radio buttons to set the origin of the stock to the center of the stock, this is very important so double check. Set the dimensions of the stock as previously prepared, measure the thickness of the stock exactly using a caliper. Make sure the top of the stock is selected as Z-zero.

For the first step in the milling process a roughing step will be used. This uses a “larger” end mill to roughly cut out the model from the stock. The diameter of the mill does not matter, in most cases it will even be the same as the finishing mill. For the example a 6mm end mill will be used for the roughing process.

The machining margin around the model should be set to minimal the size of the roughing mill so it can remove material around the model. Set the cut plane to the center of the stock, the over cut value is the one to set correctly. This value specifies the distance the mill can be lowered beneath the cut plane to clean out material in pockets for example. To define the value you need to calculate the distance between the cut plane and the bottom of any pockets that can only be milled from one side.

Set the overcut value

If no over cut value would be used in the example the part will not be milled correctly on the sloped sides. The top will be milled making a nice sloped side but when the bottom is milled the mill can only go as far as to the edge of the backside of the part, the small triangle of material can not be removed. By specifying an over cut value of approx 1mm the top side will be milled away until the red line and the back side to the blue line. The top pass will completely mill to full sloped side while the bottom pass will mill “air”. Increasing the over cut value will not damage your part, it will only increase milling time since the mill needs to be plunged deeper in the stock many times during the finishing pass.

Step 2

Click on the Add Tabs button to add the tabs that hold the model in place during the milling process. These tabs must be strong enough so they don’t bend when the mill is plunging in the stock. They must also be wide enough to prevent the part from shifting sideward in the stock when the mill is moving from left to right. Increasing the size of the tab or adding more tabs will solve this but all these tabs need to be manually removed at the end of the process.

The number and location can only be defined on feeling. Most forces will be in the X-direction during the finishing process so as a rule of thumb set the width of the tab to 50% of the finishing mill and the height of the tab to 50% of the width. Click on the Add tab button and move the mouse over the model. A pipette appears were a tab can be added, clicking the left mouse button will add the tab.

When the location of the tabs are set, each tab must also positioned in the z-direction. In order to do this, click on the tab in the Edit tabs list. Rotate the model by pressing and holding down the left mouse button while moving the mouse until you have a good view of how the tab is attached to the model. Use the slider to move it to the top or to the bottom until it is positioned to your own preference. The Z-position of the tabs don’t need to bee all at the same height, however keep in mind that the over cut value is large enough to remove the material up to the tabs. Press the close button and adjust the value of the over cut before pressing the next button.

Set the tabs

The roughing tool path cuts out the part roughly from the stock. Enable the roughing tool path by checking the Create roughing tool path checkbox. To select a mill for this tool path press the Select button, this will display the tool database.

The tool database

The amount of tools will vary, in above view all default tools were deleted and the most used tools are newly created. If you create a new tool, provide a logical name for this, select the tool type and specify the diameter of the cutting head (not the shaft). The distance that the mill will be advanced every pass in the Z-direction is specified by pass depth, for the X- and Y-direction this is specified by the step over value. Typical values for pass depth is 50% of the cutting head diameter, for the step over this is 33% of the cutting head diameter.

The spindle speed is only needed in case the CNC machine can handle this although it is good practice to set this value as a reminder during the milling process. In this case the speed can be manually set based on this value in stead of calculating it again. Typical speed for aluminum can be calculated using the previously mentioned formula RPM = 50000 / Diameter.

The feed rate is the speed the mill will move in the X- and Y-direction during the milling process. This speed is defined by many variables like RPM, mill bit material, force of the machine, number of cutting flutes and so on. Using HSS 8%Co 3 flute bits and 3500 RPM (maximum of the machine) for POM this can be 200mm/min and for aluminum 100mm/min. Plunge rates are a bit less, 150mm/min for POM and 50mm/min for aluminum.

These are reference values, there are all kind of formula’s on the internet but bottom line is that you will need to define the optimum settings for your self. Use a small piece of scrap material and do experiments. For this the Input field on the MDI Alt2 tab is very convenient using G01 X… Y…. Z…. F…. commands where the F defines the speed in mm/min. A good feed rate is when small chips are produced and the mill and mill bit makes a nice homogeneous spinning noise. If powder is produced in stead of chips or than the speed can be increased, if you hear a crunching sound and feel a lot of vibration the speed must be decreased. Start with low speeds (50mm/min) and increase with steps of 25mm/min until you find your optimums.

The tool number is used to indicate the tool in the CNC machine in case multiple mills can be placed and the machine can automatically change the mill. Select the mill that will be used for the roughing process and click the OK button, this will copy all values of the mill selected.

During the milling process the mill will move rapidly from one position to another if a part of the stock does not have to be removed. This is similar as using the G00 command, the minimum distance between the stock and the mill can be set by the rapid clearance gap, 2mm is a good default value.

The machining allowance specifies how much material must at least remain around the model, this will be removed during the finishing tool path, here a value of 1.0 mm is a good default value. Cut3D will warn you if selected values are outside an optimal range, if so don’t ignore the warning but adjust the parameters.

Select the Z-level strategy, select the X-direction and set profiling to none. Roughing means cutting the stock in a rough shape of the model, although profiling and 3D raster options are nice options for finishing they only increase the milling time at this point.

Press the calculate button to generate the tool paths, when finished the blue lines indicate the path of the mill during the milling process, the red lines indicate rapid movement of the mill to different locations. You can switch between the top and the bottom view by pressing the Side displayed… radio button.

Step 3

A similar process is used for generating the finishing tool paths. Select a mill that will be used for this process. When sharp edges are required, this needs to be an end mill, for curved area’s this needs to be a ball nose mill.

The step over value is an important value to set. Since Cut3D finishes by moving the mill from left to right, than advance the Y direction a bit and move the mill from right to left perfect circles can never be milled since there will always be some remaining material. By setting the step over value to a very small value (0.1mm or 0.2mm) this remaining material is limited, however it increases the machining time rapidly. A feature request for a “pencil” cleanup has been submitted to Vectric similar to the profile option in the roughing tool path. This “draws” a circle in which case all remaining material is removed and the step over value can be kept to a typical value of 33%.

The raster angle specifies in which direction the mill will pass over the part, by adding the a second pass 90 degrees to the first there will be even less remaining material but the machining time doubles. For the example a single pass along the X-direction is sufficient.

Press the calculate button to calculate the tool paths, this might take a while. Also here the blue lines indicate the path of the mill during the milling process, the red lines indicate rapid movement of the mill to different locations. You can switch between the top and the bottom view by pressing the Side displayed… radio button.

Step 4

Press the next button, this will show the Cut Out Tool path which is used to separate the part from the stock. This is better done manually so disable the checkbox and press the next button to simulate the tool paths.

Never skip this step. This step allows you to see the final part without wasting hours of machining time and material. If something is not set correctly (like over cut) you will be able to detect it here and go back to change it.

Select the top side to be displayed and click on the Roughing Tool path Preview button. Check if the result is according your expectations. Than select the bottom side and click the Roughing Tool path Preview button followed by a click on the Finishing Tool path Preview button. Select the top side to be displayed and click on the Finishing Tool path Preview button. Both the top and bottom side should look how you expect them to look.

Step 6

In order to process the tool path in Mach3 select the Mach2/3 Arcs (mm) (*.txt) post processor. Select the top in side displayed… and click on the Roughing Tool path Save button. This will prompt for a filename, add a logical part name in front of the suggested filename and the top roughing tool path will be saved. Click on the Finishing Tool path Save button, use the same logical part name in front of the suggested name.

Step 7

Repeat the process for the bottom tool path by selecting the bottom in side displayed… Use again the same logical part names, in total there should be four files created. When finished, save your file before closing Cut3D so you can change settings in case the final part is not what you were expecting.

And finally we are ready to load the G-code in Mach3 Mill and mill the part.