Category Archives: CNC

Changing Spindle Bearings on a Taig CNC Mill

The spindle on my Taig CNC mill was getting uncomfortably hot after a few minutes of milling; especially at higher RPMs. It ran smoothly and without any play, but with a noticeable friction, so I decided to try to change the ball bearings.

Taig CNC mill

Ball Bearing Selection

The bearings have the standard dimensions 17x40x12 mm (inner diameter x outer diameter x width) and this apparently is designated with the number 6203 in the ball bearing world.

I am not a mechanical engineer and have little knowledge of the intricacies of ball bearings and it was also surprisingly hard to find a lot of good information online on how to select the proper bearings for the application. I wanted high quality to avoid having to change them soon again and I thought that dust covers would be a good idea to minimize the risk of chips getting into particularly the lower bearing. After some browsing of an online catalog (at, although there are countless others), I realized that there were plenty of options, even after selecting a particular well respected brand. It was clear that deep groove bearings were required since they can handle axial loads as well as radial ones. Since rubber seals were slightly more expensive than metal shields, I thought they were superior and bought two SKF 6203-2RS bearings. This unfortunately turned out to be less than ideal.

After replacing the bearings (the process I used is described below), it turned out that the spindle still rotated with quite a bit of friction. The rubber sealed bearings themselves did indeed have significant friction, which was concerning even before putting them into the spindle, but it became even worse after the assembly was done. A quick test run revealed that the spindle got at least as hot as before and that the motor was almost not powerful enough to even run the unloaded spindle at full speed at the highest gear.

I  think part of the reason for the high friction was the rubber seals, but since it got even worse after assembly, I think there is also another part of it. It must be either that the bearings  are put under radial stress in the spindle, compressing them tighter and thus causing them to run with higher friction, and/or that there is ever so little misalignment  between the two bearings.

So, back to the bearing catalog. This time I tried to address both of the reasons for the high friction. I opted for bearings with a higher play, designated by the option C3. I also selected an unshielded bearing for the top one (6203/C3) – which will hopefully not be subjected to chips or other debris – and metal shields for the lower bearing (6203-2Z/C3). This worked much better and now the spindle runs smoothly with very little friction and no discernible play.

Below is a description of how I replaced the bearings the second time.


I first removed the spindle motor. It is fastened only by two screws holding its mounting plate to the rest of the spindle.

The spindle is secured to the Z-axis assembly by a single set screw holding on to a dove tail, so this was easy to remove.

Spindle removed from mill

The pulley is secured by two set screws. I released them and gently applied some force to pull it off from the shaft. There probably are some good special tools for this, but I used two screwdrivers as levers.

Removing the pulley

Under the pulley, there is a nut (with a very fine thread) that needs to be removed. I held on to the shaft by one wrench on the lower side while using another to loosen the nut.

Removing the nut

Now the shaft had to be pushed out of the bearings. This takes a lot of force. Maybe there is some trick that I am not aware of. Using a mallet to hammer it out might be one option, but I initially tried to be more gentle by using clamps (more than one was required to two get enough force) together with wooden blocks to avoid damaging the shaft. If I had had a gigantic vise with a wide enough mouth, that would probably have been a better option.

Pushing out the shaft using clamps and wooden blocks

Once the shaft was fully pushed into the top bearing, I resorted to hammering on a dowel at the end of it.

Hammering out the shaft using a dowel

This was successful.

The shaft has successfully been removed.

The next step was to remove the bearings. Here I came up with an (in my opinion) clever method. The housing is made of aluminum and the bearings are obviously made of steel. Aluminum expands a little more when it is heated than what steel does, so by heating the whole thing up by a few tens of degrees, it should be much easier to remove the bearings. So I set the kitchen oven to 60 C and let the spindle cook for an hour or so.

Cooking the spindle

This was even more effective than I had thought. The bearings more or less fell out by themselves.

Bearings falling out of hot spindle.

There were a few shims between the ends of the bearings and the spindle, probably to prevent the inner ring of the bearings to touch any part of the housing.


Before the housing cooled down, I inserted the new bearings into it (together with the  shims).

Upper bearing without shield or seal

Lower bearing with metal shield

Inserting the shaft into the new bearings was a bit hard. I probably should have heated up the new bearings before attempting this. Instead I lubricated the shaft a little (not sure this helped) and used force in the form of a hammer to hammer it in. Maybe this could harm the bearings due to the high axial load, but fortunately the spindle ran fine afterwards, so perhaps it was no big deal. Next time I will probably heat the bearings (and perhaps even cool the shaft, although I am worried that might cause too much condensation and then rust) before trying to force it in.

Hammering in the shaft

After making sure the shaft turned smoothly with little friction and with no discernible play, I replaced the nut (not tightening it very hard as that increased friction), added the pulley and then put the whole thing back onto the mill.

The shaft and its nut are back

Reassembled Taig CNC mill

So despite the unnecessary set of sealed bearings I bought and having to do it all twice, I am pretty happy with the bearing replacement. Now the mill runs fine without the spindle getting hot, even after long runs at maximum RPM.

Another try at PCB depanelization

I tried to separate the PCBs on another panel using the CNC mill. Here is the report on how I did it (so that I remember until next time).

The PCB panel

The first step is to have a CAD drawing in DXF format of at least where the center lines of all the cuts shall go. It is not obvious how to best lay out these lines. Should one go for fully separated PCBs? Or should one leave bridges between them to avoid the problem of PCBs (maybe) flying around as soon as they are separated, but with the problem of not getting fully separated PCBs in the end?

This time the PCBs were super-small, only 10.5 mm x 6 mm, so I decided that the holding force of the double sided tape would probably not be strong enough to securely keep the PCBs in place. Therefore I opted for only partial depanelization by milling. Since the thickness of the PCBs in this case was only 0.6 mm, I could use scissors for the final step. In fact, I could have exclusively used scissors and not involved the mill at all, but that would not be as fun. And one could argue that that would have resulted in more warping and strain on the PCBs.

To define the mill pattern, I exported data in DWG format from the CAD program (Altium) and opened it in DraftSight where I made some adjustments. After this, the CAD files contained the center lines of the mills, the board outline and the outlines of the holes in the panel. I then saved it as a DXF-file, as Fusion 360 (where I create the G-code program for the mill) does not seem to understand DWG.

In Fusion 360, I started a new sketch and used the command INSERT -> Insert DXF to import the CAD file.

DXF import dialog in Fusion 360.

Here one can select which layers to import and what units to use. In my case I only needed the data on layer MECHANICAL8 and the units were (of course) millimeters.

When the data is in, one does not have to do any more work in the MODEL section of Fusion 360, but there is more to be done in the CAM section.

Add a new setup (SETUP->New Setup) and make appropriate selections. One important thing is to define the origin in a clever position that is easy to identify and calibrate on the mill. For this purpose I had placed a 3 mm hole in the panel which I intended to locate using the 3 mm end mill needed for the depanelization (2 mm would probably have been a better idea, but I do not currently have a suitable 2 mm end mill). For some reason, Fusion 360 refused to select the center of the 3 mm circle as the origin until I first placed the origin at the end of a mill line and then retried to select the circle. Weird bug.

Defining the origin as a Sketch Point

In the Stock tab of SETUP I selected Relative size box, No additional stock and Round Up to Nearest 1 mm. This is probably unimportant since there is not even any 3D body defined, so Fusion 360 thinks the model has zero size.

In the Post Process tab, I added a suitable Program Name and Program Comment (helps with default file name and comments in the G-code).

The main trick is to use 2D contour with Compensation Type set to Off as the milling strategy in order to let the center of the mill follow the center of the lines in the drawing. This is done by 2D->2D Contour:

Adding a 2D contour milling pass

I selected the appropriate tool in the first tab (in this case a 3 mm end mill) and in the second tab I selected all the vertical segments. This is a bit tedious since drag-select does not work. The reason I only selected these segments and not the horizontal ones, is that I want the panel to stay as rigid as possible as long as possible:

Selecting all the vertical segments in the first 2D contour pass (not all segments have yet been selected above).

In the third tab, I define the heights. I generally decrease the clearance and retract heights to make the machining faster. I let the Top Height be 0 mm from Stock top and set the Bottom Height to -1 mm from the Selected contour(s) (Stock top would also have worked). This defines that the tool will go 1 mm deep (when I zero the mill on the top of the PCB), which is enough since the PCB panel is 0.6 mm thick.

Defining heights

The fourth tab is very important. This is where Compensation Type shall be set to Off so that the center of the mill tool is not offset from the lines:

Set Compensation Type to Off.

The fifth and final tab is also somewhat important. Here we need to untick the Lead-In and Lead-Out boxes to avoid undesired lateral movements of the mill that would ruin the PCBs. I also unticked the ramp box and let the tool plunge straight down:

Untick Lead-In and Lead-Out.

After clicking OK, the following tool path (yellow) was generated:

First tool path, vertical cuts

Fusion 360 reorders the segments in some more or less optimal order. The order in which the segments were selected does not seem to matter.

Duplicate the operation (to avoid a lot of repetition of settings), clear which segments are selected and select the horizontal lines:

Selection of horizontal segments

The resulting tool path looks like this:

Tool path for horizontal segments

As I mentioned, the reason for having two operations is that I wanted to mill the short segments first (to keep the panel as rigid as possible as long as possible) and with a single setup, it is impossible to control the order of the milling.

To generate the G-code, click on the Setup containing the two milling operations (so that not just one of the milling steps is selected) and then select ACTIONS->Post Process.

Fusion 360 has an irritating habit of forgetting the post processing settings when it updates itself. This results in the following error message:

Stupid post processing error message after Fusion 360 has updated itself.

Since the previous configuration has been forgotten, I have to tell it again that I do indeed have a Mach 3 mill and (very importantly) that it should not use the commands G28 and M6.

Important settings for my mill.

After the G-code has been generated (by clicking Post), it is finally time to set up the mill to do the work. I had designed the panel such that it had four 5 mm holes that fit with the T-slots of the milling table. I drilled corresponding holes in a piece of sacrificial MDF board and placed double sided tape on the board:

MDF with holes matching the panel and double sided tape.

I then put down the PCB panel on the tape:

The PCB panel has been attached to the MDF board.

It is then time to screw the panel to the table while making sure the panel edge is very parallel to the table. I had to use oversize (M6) nuts under the heads of the screws to make them fit with the T slots:

Panel in the mill.

I manually moved the mill precisely to the 3 mm hole on the left edge of the panel and zeroed the coordinates. Then it was time for action:

Milling the vertical slots.

Milling the horizontal slots.

Milling finished!

Using a pair of scissors, I cut the PCBs apart.

Individual PCBs

The result is acceptable, but not perfect. There are some burrs, which may have been caused by the end mill not being as sharp as it should have been. At first glance there seems to be a bit of mis-registration of the milling compared to the PCBs, but at least some part of  this is actually mis-registration between the overlay print and the copper. Compared to the copper, the milling seems to be very well positioned.

An idea for future improvement that I have is to not just leave a bridge between boards, but make this bridge thinner by milling down partially through the laminate. Maybe one can get away with leaving 0.3 mm or so of the material. This would make the scissor cutting easier. It is probably best to make these partial depth mill cuts first when the tape is pristine and let the full depth cuts (which can tear the PCBs somewhat loose from the tape) follow later.

Improving the Depanelization Process

In the previous post, I wrote about using my CNC mill to depanelize PCBs. One issue  I had was that the boards were not cleanly separated from the panel since they moved away as soon as the mill broke through the tab connecting them to the panel, leaving a pointy feature.

I tried to improve this by using double sided tape to keep the boards in place:

Double sided tape on the CNC bed to keep the sacrificial board firmly in place.

The sacrificial (MDF?) board on top of the tape. The glossy surface will make it easier to remove the tape.

The PCB panel has been secured in place. There is double sided tape between it and the board. Two clamps aid in the workholding.

Milling in progress. Some boards still get loose, but some stay in place.

Separation of the upper three rows of boards complete.

The mill is not big enough to reach all boards in one setup and I tried to reuse the tape when separating the lower two rows. Due to the dust from the initial milling getting into the adhesive, this was not a great idea. Using new tape would have been better.

The sacrificial board after the panel and the top side tape have been removed. The board can be reused. The pattern created by the mill can be used to position the next panel. Even better would be to have guide holes in the PCB panel and run a mill program to create corresponding holes in the sacrificial board to aid in precise positioning of the panel.

In summary, using double sided tape to aid in the workholding is a promising idea. With the small board in this panel it was however only semi-successful since the adhesive has very little area to attach to and the PCB surface is a bit uneven due to the trace pattern. On larger boards it will probably work better.