Introduction
This wiki outlines the induction exercise for using the Imes-Icore M40 3-axis router which is situated in the E28 workshop in heavy engineering, Cockcroft Building. Note that the induction only includes cutting .dxf files (i.e. 2.5 axis cutting).
In the induction you will machine a small 6 mm comb.
here is the latest solidworks file: 6MM_COMB_1.3
The slots on the comb vary in size from 5.8, 5.9, 6.0, 6.1 and 6.2 mm to give various degrees of fit when assembled with another 6 mm piece. Note also that the chamfers vary in size to help locate the part when assembling. A variety of dogbone shapes have been used to show how these can look on your part.
The induction covers the following steps:
- Using the Cut2D software to generate G-code
- Setting up the 3-axis router
- Using the Remote software to setup and control the CNC router machine
3-axis CNC router in E28
The specifications of the E40 machine (link to full spec) are as follows:
- cutting volume 1000 x 900 x 250 mm (XYZ)
- typical accuracy 0.03 mm
About this wiki
It is expected that you should all take part in updating the wiki documentation in any ways that are suitable (during or after the induction, not before!). We want this to be an amazing, clear, detailed (but concise) set of documentation that we can roll out to other years and use in future years. Note that all amendments are logged, so only make corrections that are absolutely correct. We will discuss
1. Using the Cut2D software to generate G-code
Open Cut2D from the desktop.
Cancel the register request for the software (if asked).
File > open (find the 6MM_COMB_latestversion.dxf file in the DP402 CNC induction folder on the desktop).
In the job setup tab (also Edit > job size and position):
- specify workpiece size, i.e. 150 x 120 mm (for this induction)
- specify material thickness as 6mm
- z zero should be on the bottom of the material (this is important!)
- XY origin position should be bottom left (this is important!)
- don’t use origin offset (uncheck this box)
- don’t use any data scaling (centre or scale)
- units: mm of course!
- click OK
In the drawing tab (on the left):
- Remove text from below design relating to “`Solidworks Student License”
- select lines that form boundaries (e.g. internal slot) and click join open vectors. This joins them together so they will be cut in a single process. Then do the same for the external contour.
- move the part (all together) into the middle of the workpiece, remember to allow space for the fixings and for tool clearance around the outside (draw a test circle to represent cutter and move around your work if needed)
In the toolpaths tab (on the right, we recommend pinning this up using the drawing pin icon):
- material setup: z zero (bottom), t = 6 mm, rapid clearance = 100 mm, home = (0,0,100 mm) (XYZ)
Create pocket toolpath (inside)
- select the single joined line that define the internal pocket
- click create pocket toolpath
- start depth: 0 mm
- cut depth: 6 mm
- tool setup: edit (the settings below are for this exercise)
- tool diameter: 6.0 mm – ensure that this is correct for the tool in the machine
- pass depth: 2 mm
- stepover 2.0 mm
- spindle speed: 14000 RPM
- feedrate: 40 mm/sec
- plunge rate 15 mm/sec
- click OK to accept the tool setup
- click calculate your toolpath
- close the preview window
Create profile toolpath (outside)
- click create profile toolpath – check the Outside/Right radio button
- start depth: 0 mm
- cut depth: 7 mm (material thickness + 1 mm – the extra 1mm is to ensure the tool cuts all the way through the work piece cleanly)
- check the Conventional radio button (to indicate cutting direction)
- tool setup: edit (settings need to be the same as above)
- check the add tabs to toolpath box
- click edit tabs to then select where on the profile (outline) you want to add the tabs
- length: 10 mm
- thickness: 4 mm
- click calculate your toolpath
- close the preview window
Preview all toolpaths and check that it is doing what you expect
While still in the tooloaths tab, save toolpaths using: processor ISEL Arc (mm)(*.ncp) file type.
Your file should be saved in the ‘DP402 CNC inductions‘ folder on the desktop and should include the module, group number, date, e.g. be DP402_group2_08_11_2019.ncp
2. Setting up the 3-axis router
- press power button on computer (if not lit already)
- press start button on computer
- hold down cover button then open the doors
- make sure the bed is flat (you may need to lightly sand this) and ensure there is no debris/dust (you might need to use the hoover)
- position your workpiece against the XY datum making sure it’s the orientation corresponds to how you’ve set it up in the software (ideally 150 x 120 mm, X x Y mm)
- screw in your workpiece in two opposing corners (leave plenty of room for the cutter)
- close the doors
3. Using the Remote software to setup and control the CNC router
Open Remote from the desktop
You should now be prompted by the software to carry out a reference run where the machine will return home (Press CTRL + Z to do this if the software doesn’t prompt you to do it)
Open your .ncp file that you saved earlier.
Click the Display graphic of current file icon (it looks like a graphical display)
In the menu, go to Window > Tile horizontally (to show both the cutting toolpaths and the g-code together)
Ensure that the machine speed is set to 5% or less (in the bottom part of the window). This can be adjusted during the cutting process to ensure a safe cut – you can also press the 0 button to stop the cutter. This is important!
click START: Output file in automatic mode. This is the green (1) button and will start the machine and it will start moving towards the workpiece.
Once the machine has finished and moved back to the reference home, you can hold down cover button then open the doors.
Use a vacuum cleaner to remove all dust and debris then unscrew your workpiece from the bed.
Carefully remove the part from the workpiece with a chisel and hammer, bandsaw, Dremel or another appropriate tool and debur your part (with sandpaper) as necessary.
