[alank2]

Hi Everyone,

I recently got a Microcarve MV3 and have been playing around with it. I also have a SuperPID so I can control the router RPM. My router however is a cheap trim router from harbor freight (2.4amp). I noticed that it spins CW (perspective = top looking down on it) so that is my first question - is there a "standard" direction that routers spin and most bits are designed for, CW or CCW?

I was building a fixture tonight from some 1/2" plywood scrap and the number one problem I ran into is one of when doing multiple passes, the passes are not the same size. For example, I cut 0.125" passes and the top of the rectangle is bigger than the bottom of the hole. Holes do the same thing, larger diameter at the top, smaller at the bottom. I tried 25 and 50 IPM, 15K and 30K rpm. I am using this bit, which is also from harbor freight:



How can I make cuts in multiple passes where each pass is the same size?

edit - I forgot to mention that my cutting method is where the Z is constantly plunging at a rate that makes it 0.125" lower for each pass, so it is always plunging (very slowly) and moving in a rectangle or circle at the same time. This looks like a spiral for a circle for example. I could change to a method where I plunge to -0.125 and then cut that rectangle or square, then plunge again, then cut, etc...

Thanks,

Alan

[ger21]

- is there a "standard" direction that routers spin and most bits are designed for, CW or CCW?

Yes, CW.

Sounds like you're getting machine flex, but it's really hard to say. It looks like your bit is pretty dull. 15,000 rpm is probably good for up to 100ipm with that bit (if it were sharp). At 25ipm, 8000-1000 rpm would be better, and the bit would stay sharp longer.

Personally, I think that any bits from Harbor freight are probably junk to start with.

How can I make cuts in multiple passes where each pass is the same size?

Use sharp bits (carbide), in a decent router with minimal runout. Make sure the machine isn't flexing. If it is, take shallower passes.

[alank2]

Hi Gerry,

I've been trying things and one thing that makes a big difference is whether I cut the rectangle in a clockwise direction or in a counter-clockwise direction. The rectangle seems to have its straight lines bow somewhat outward when going clockwise and ever so slightly inward when going counterclockwise. Does this make sense? Is there a direction you are supposed to cut (CW or CCW)?

Thanks,

Alan

[alank2]

Hi,

A picture of cutting in both directions (starting in the upper left and moving CW or starting in the lower right and moving CCW):



Is the CCW a "climb" cut and the CW a conventional? It does the same thing in plywood as the above picture. It is almost as if the bit is "pushed"...

Thanks,

Alan

[ger21]

Is the CCW a "climb" cut and the CW a conventional?

Depends on whether it's inside or outside, but I'd say yes in this case.

If the machine has some flex, a conventional cut will tend to cut extra material as the bit is pulled into the wood.
A climb cut will tend to cut less, as the bit is being pushed away from the wood.

If your depth of cut is .025", I'm guessing the bit is extremely dull.

[louieatienza]

Depends on whether it's inside or outside, but I'd say yes in this case.

If the machine has some flex, a conventional cut will tend to cut extra material as the bit is pulled into the wood.
A climb cut will tend to cut less, as the bit is being pushed away from the wood.

If your depth of cut is .025", I'm guessing the bit is extremely dull.

To add to this, you can do your pocketing with climb cuts, and leave .01" or so for finishing. Then you can do a finish pass using conventional cuts. The climb cut will leave your part with a slightly minus tolerance, and when yo do the finish pass, there won't be enough material cut to "pull" the bit in considerably.

As for the bit, looks like the tip is discolored from excess heat. You can try a single-edge spiral "O"-flute bit at the same RPM or a little higher, with more cut depth per pass.

As for climb vs. conventional: climb cutting is when the bit is rotating in the same direction as the tool, as if the bit was a tire rolling on the road; conventional cutting is when the bit is rotating opposite the tool direction.

[alank2]

Hi,

To add to this, you can do your pocketing with climb cuts, and leave .01" or so for finishing. Then you can do a finish pass using conventional cuts. The climb cut will leave your part with a slightly minus tolerance, and when yo do the finish pass, there won't be enough material cut to "pull" the bit in considerably.

As for the bit, looks like the tip is discolored from excess heat. You can try a single-edge spiral "O"-flute bit at the same RPM or a little higher, with more cut depth per pass.

As for climb vs. conventional: climb cutting is when the bit is rotating in the same direction as the tool, as if the bit was a tire rolling on the road; conventional cutting is when the bit is rotating opposite the tool direction.

Thanks for the great ideas everyone. I think I'm getting more of it now. I've been doing some reading about rpm, chipload, etc.

So if you are merely cutting a straight line - one side of the line will be a climb cut and the other side will be conventional, right?

Thanks,

Alan

[ger21]

So if you are merely cutting a straight line - one side of the line will be a climb cut and the other side will be conventional, right?

Yes

[alank2]

Hi,

Ok guys, I had a light bulb moment tonight. For some reason I was thinking that cutting was done with the full diameter of the cutting tool, but this would lead to both a climb and conventional cut being done at the same time. After thinking about this it occurred to me that you probably only want to cut the material at 50% of the cutting tool diameter. I then looked at the pocket wizards in mach3 and noticed they show a stepover of 20%! Am I on the right track here?

Thanks,

Alan

[ger21]

If you're cutting out parts, then typically, you will use the full diameter of the tool.

With wood, when pocketing, I'd cut at 75-90% stepover, in order to get done faster. You need to use slightly less than 100% just to have a small amount of overlap.
If your machine isn't rigid enough, you may get better results with a smaller stepover, which requires less force.

From my experience, when cutting wood, conventional cutting will almost always give better results. I only use climb cutting to prevent or minimize tearout or chipping.
Grain direction can have more to do with whether to climb cut or conventional cut than other factors.

[louieatienza]

Hi,

Ok guys, I had a light bulb moment tonight. For some reason I was thinking that cutting was done with the full diameter of the cutting tool, but this would lead to both a climb and conventional cut being done at the same time. After thinking about this it occurred to me that you probably only want to cut the material at 50% of the cutting tool diameter. I then looked at the pocket wizards in mach3 and noticed they show a stepover of 20%! Am I on the right track here?

Thanks,

Alan

I think it depends on the material you use, the power of your spindle and machine, the depth of cut, and the ridgidity of your setup. Most wood and wood products are pretty free-cutting and you can use a larger stepover. Your spindle, steppers, or mechanical components may or may not be up to the task of taking larger stepovers, you may need to make adjustments based on the particular material. Your stepover (radial depth of cut or rdoc)can be affected by your axial depth of cut (or adoc). Usually the deeper the adoc, the less the rdoc. Also the lower the rdoc, the higher the feedrate you can usually set. You may actually have a higher material removal rate by going deeper, with less stepover but more speed. As for ridgidity, I generally find it best to climb cut if the setup is ridgid enough - larger diameter tool, smaller flute length, less Z travel. Since the tendancy is to push the tool away it can lead to more vibration. Since convevntional cutting "pulls" the bit into the work, it can actually "pull" in the direction of less ridgidity or backlash to "tighten up" a system. This is how some machinists compensate for backlash in a manual mill or tool compound on a lathe.

In your examples above, it might even be better to use a larger tool to hog out the material using a spiral offset pocket, then come back with the smaller tool to run n inside profile cut to bring the part to final size. With the larger tool you cna be more aggressive. Using a tiny tool to pocket is asking a lot of the tool, and with the tiny adoc, you're just burning and dulling the tool tip, basically burnishing the pocket floor.

[orkki]

To me it looks your bits are left hand twisted.

[louieatienza]

To me it looks your bits are left hand twisted.

It's a downcut spiral! Maybe switching to an upcut spiral will help out as well since it will help with chip removal....