Tips for the Proper Use of Tools

Always choose a milling cutter which is suitable for the material which you process. Please notice our extensive descriptions of the tools and their fields of application. Withstand the temptation to use a tool which you have at your fingertips incidentally. The tool should be as short as possible and be clamped as deep as possible into the collet chuck.

Internal contours should be milled clockwise, external contours counter-clockwise; so the worse side which has been milled in same direction will always be waste. Please note also the paragraph Milling Same or Counter Direction.

You should mill deeper slots in several steps, if possible. Usually, it is more economic to mill a slot in several steps with less dipping depth and at higher rates of feed than at once and accordingly slower. General guidelines for the dipping depth:

	foam plastic: 5 – 10 fold cutting edge diameter
	plastic (acrylic, etc.): 0.2 – 2 fold cutting edge diameter
	aluminium: 0.2 – 0.5 fold cutting edge diameter
	steel: 0.1 – 0.3 fold cutting edge diameter
	stainless steel: 0.05 – 0.1 fold cutting edge diameter

In any case, the tool should be cooled if possible. The best way of cooling is with a spray lubricant or – better than nothing – with compressed air.

You will find further information on cooling here.

Setting the Operational Parameters

Whether it is actually possible to work with theoretically determined values for rotational speed and feed rate depends on the interaction of a number of factors:

	what material is the workpiece made of?
	type of coolant/lubricant
	power/maximum rotational speed of the spindle
	minimum/maximum feed rate of the CAM system
	stiffness of the machine.

As there is a large number of possible system configurations, these values can only serve as clues. They are maximum values which are calculated for optimum external circumstances for which we cannot assume liability due to the abovemen- tioned numerous configuration possibilities. You should approach these values from the safe side, i. e. you should choose at first for most materials a lower lowering speed, dipping depth and feed rate – but keep up the rotational speed. During the milling process, you can further optimise the results by carefully changing the parameters.

If the calculated feed rate should be faster than your CAM system can actually move, you should set the maximum speed of your system as feed rate instead. However, you should reduce in this case the rotational speed of the spindle a little bit.

The dipping depth depends on the power of your spindle, i. e. only if your spindle has a sufficient power reserve, you may actually set the maximum dipping depth. In case of doubt: It is better to remove in more steps less material than too much at once. If you are not sure about the correct dipping depth, you should also reduce the feed rate. Depending on the construction of the machine, you should observe the following rule of thumb: when using lightweight construction machines (e. g. vhf CAM 100–CAM 2040), you should reduce the removal rate, when using heavy machine tools, you should rather reduce the feed rate.

Please observe also the load display of the spindle controller, especially when you are working with bigger tool diameters on difficult to machine (hard) materials like stainless steel. It should not exceed a load of 80%, if possible. So you should approach the specified dipping depth only stepwise and watch always your spindle load.

Milling Same or Conter Direction

The quality of both milled edges of cut will never be exactly the same. While milling in the counter direction, the tool moves – relatively regarded – against the material. The chip size becomes increasingly bigger towards the middle. While milling in the same direction, the tool moves with the material; the chip size is reduced again until the exit of the cutting edge from the material. The cutting edge runs in the counter direction as well as in most parts of the same direction against massive material. However, immediately before the exit, there is not much material left. So the last bit will often be rather torn off instead of being cut cleanly. Therefore the counter direction becomes smoother than the same direction. However, this effect varies strongly with the characteristics of the material, the geometry and sharpness of the milling cutter and the operational parameters.

Thus we recommend to mill internal contours clockwise and external contours counter-clockwise.

What to Do in Case of Problems?

	If especially plastics should melt, the reason may be that the tool advances too slow and produces too much heat. Please reduce the rotational speed and increase the feed rate at the same time.
	If a milling cutter should become plugged, usually the chips have not been discharged quick enough. In such a case, the dipping depth and/or the feed rate have to be reduced. It may also help to use a different tool. Please note the hints on the number of cutting edges of milling cutters.
	When working on critical materials like extruded acrylic, milling cutters with polished flute have proven to be well suitable. Here the chips can hardly stick to the cutting edge.
	In case of a burr formation, you should increase the cooling. It could possibly become necessary to make also an additional finishing pass.
	If a tool breaks rather frequently, the removal rate is too high or the true running of the spindle is not exact enough. Please reduce in such a case the feed rate and/or the dipping depth and exchange the collet chuck for test reasons.
	If your material should not be listed, please classify it according to its machinability (hardness). When working on brass for instance, you should rather orient on the parameters of aluminium than on those of stainless steel, whereas when working on construction steel, you should rather orient on stainless steel than on aluminium.
	In case that your controller does not have a real look-ahead function (point-to-point or look-ahead of just one vector), you should stay below the calculated maximum feed rate, especially when performing fine engraving works. For instance, if you engrave small fonts which consist of numerous little vectors, the machine always has to accelerate and slow down strongly again. Even if the controller calculates one vector in advance (e. g. vhf CNC 450), it cannot accelerate in a curve to maximum speed because each next but one vector will be “in the dark”. You have a similar situation when you drive with your car in the fog, when you can only see from one guiding pole to the next. So an optimum velocity along the path (as is the case with CNC 550–980) can only be achieved with limitations. The bearings of the machine and the tool will be exposed to strong forces due to the strong acceleration and brake applications. On top of that, the machine can “overshoot” due to the mass inertia. This effect becomes obvious in a bucking of the machine which leads to results that are worse on the whole. The speed advantage can be neglected. Please interrupt the output process as soon as the machine starts bucking and restart it at reduced speed.
	If a higher feed rate than your system permits would be possible according to tool and material data (please note also the abovementioned remarks concerning fine engraving works), you should reduce feed rate and rotational speed accordingly.

to the top