8. Computer controlled machining

About the router

In out lab we have a TechSoft routerCAM 1224, it can take a full sheet of material stock 8ft by 4ft / 1220mm by 2440mm.

• Axis travel: 1220x2240x175mm
• Macginable size: 1220x2240x155mm
• Max Speed Rate: 200mm/sec
• Spindle Speed Range: 12000-24000
• Resolution: 0.05mm
• Vacumme bed

Safety

These large CNC machines can be very dangerous to safty needs to be taken seriously.

In our lab we have several safety precausions in place: - Never operate the machine alone - Wear hearing protection - Wear eye protection - Light curtain to ensure people do not enter the machine area whilst it is working on a job - Extraction for dust - Emergency stop buttons

Machine Set Up

We went through how to set up the machine before starting a job.

We turn of the two wall power switches, one for the machine and one for the extractor. Then turn on the power switch on the front of the machine. Part of the shut down procedure is to hit the emergency stop button, this makes it harder for someone ignorant of the machine to start it. So we twist the emergency button then hit the reset button.

On the pendant control we press ok to allow the machine to home the axis.

The axis of the machine: - Z is up (+Z) and down (-Z) - Y is forwards (-Y) and backwards (+Y) - X is left (+X) and right (-X)

Move the head to a easily accessable position.

We then use the two spanners to change the tool and collet if needed to match the planned job.

Good to just compare the length of the tool to the thickness of wood, gives a idea if its the correct length and how far you could insert the tool into the head. Good to leave about 1cm extra.

Tighten the tool until its just gets stiff then a extra 1/8th.

Vacuume Bed

The bed of the machine has holes which a motor pulls air through creating a downward vacuume. There is a balence needed, you dont want to completly block all of the holes with the material and plugs as you need to allow some air passthrough.

You can put down extra tubing in the channels to better match the shape of the material.

There is then a layer of sacrificial rubber that goes on to of the bed.

The vacuume has a seperate power button to the mill.

The material should be quite hard to pull up the bed.

Turn on vacuume bed when zeroing the z axis

Zero Axis

Move the head of the machine to the desired X-Y zero axis. Be aware its not too near the edge but also ensure you allow enough room for the entire job.

Hit the X-Y Zero button, You will see the X-Y numbers change to zero.

To do the z axis you need to plug in the probe to the front of the machine.

Turn on the vacuume bed as it causes the material to sag downwards a bit.

Lower the head until it is close to the top of the probe. Move the probe out of the way when lowering, just move it inwards to guage the height occasionally.

When it is about 1cm away you press the

on/off + menu

Button combination to run the probe routine. It should lower until it touches the probe then retract.

Test Cut

For my individual project this week one of the joints is a wedge joint.

I created a test model to practice milling this job and test the fit. The model includes a shallow pocket, full depth pocket, 6mm hole (for screws) and the outside cut.

We used some 18mm MDF for this job. Set up the machine as described above.

Creating toolpaths

I designed the model in fusion 360 then used the manufacture workbench to set out the jobs.

You start be going to Set up > New Setup

• Operation type = Milling
• Model = Select the bodies that will be included in your processes
• Stock mode = Fixed size box / relative sized box
• Fixed size box is useful if you are trying to fit a large project within a limited amount of stock. For example a large project on a full sheet. You set the size (1220x2440mm for a full sheet) and set a offset if you dont want it to start right on 0,0,0. Depends how well you set out the pieces.
• Relative size is useful for small projects where the stock can be just large enough for the model.
• Program name/number some machines only read numbers. The default 1001 would refer to the first process, 1002 as the second… etc.
• WCS offset, for our machine we set this to 1

You then choose which operation you need. Quite often the 2D operations are sufficient and more often than not you’ll only use the 2D pocket and the 2D contour.

2D Pocket

For use on the inside features of the model. Holes or partial depth holes.

• Tools choose the tool that is suitable for the job from those available. Larger tools can go faster because they can withstand higher forces. For the test piece we chose a 4mm flat end mill. You may need to set up a profile for a new bit as it is important it is accurate for the simulation later.
• Geometry is where you select exactly where you want pocketed. Make sure to choose the bottom edge/face of the model.
• Heights. This tab sets up the safe distances and the top and bottom heights of the job. If the pocket is going full depth we set the bottom height as -0.3mm. This allows the tool to cut cleanly through the model and just goes into the spoil area slightly.
• Passes. It is a good idea to choose multiple depths for most jobs. Large stepdowns can cause broken bits and too much strain on the machine leading to inaccurate mills. We used a 3mm depth cut.
• Stock to leave. We turned it off, but it may be useful for some jobs where dimentions need to be very accurate.

2D Contour

This has very similar oprions to the 2D pocket. - Tool. As this is the outside we opted for a larger bit, 8mm, which will be faster and stronger. - Geometry. Select the bottom outside contours.

Speeds and Feeds

Out tool base has been set up by a more experienced technician.

The basic guidlines are: - 4 meter per minute movement through material - The number of flutes increase the strength of the tool but makes it harder to eject the chips. You need to increase the feedrate with more flutes. - The diamter of the tool determins how agressive you can be with cuts. - The depth of the cut should never be larger than the width of the tool (exception of smart processes such as adaptive clearing which manages the load on the tool)

You can see the 4mm has a lower spindle speed and feedrate when compared to the 8mm bit.

4mm flatend mill

8mm flatend mill

NC Program

We use this dilogue to create the gcode which can be then sent to the machine.

It is important to choose the correct post process for your machine. We use the base Fanuc Fanuc.

Here you can combine tool paths which use the same tool so there are less seperate jobs to run.

This code is then transfered to a USB which is plugged into the Pendant.

Running a Job

Checklist: - Extractor is switched on - Vacuume bed is switched on - X, Y & Z are all zeroed - Jobs are on the USB - Correct starting tool is loaded - PPE is on - No obstructions in the way of the light cutain

Press the Run/Pause/Delete button.

Use the buttons to navigate to the correct job, likely 1001/2001.

Press ok/origin to select the job and then again to start the program.

Hover over the emergency stop until you are happy it has milled one section to the base of the material successfully.

You can see the last layer quite easily if you have tabs on the material as the head moved up and down whilst tracing the outside.

Once it is done move the head out of the way. Hoover up any extra chips. Change the tool if needed for the next job. REZERO THE Z but leave the X-Y zeros the same so that the jobs line up.

Clean Up

We use a stanley knife to cut through the tabs then a chizel to move them from the parts.

The Test Piece

It milled it out quite nicely however it did point out two main issues.

• We had not compensated for the wood being just over 18mm, 18.3mm, so the joint did not pass through.

• We need bog dones on the inner corner of the tab in the joint as it could not sit flush to the wall overwise.

You can see the final result of my project on the individual page.