New 6040 owner looking for advice from others with a chinese 6040/3040

[Boyan Silyavski]

No problem, glad that i can help here.

Here are some more tips:

1. Using the formula

Formula to determine feed rate[edit]
This formula[10] can be used to figure out the feed rate that the cutter travels into or around the work. This would apply to cutters on a milling machine, drill press and a number of other machine tools. This is not to be used on the lathe for turning operations, as the feed rate on a lathe is given as feed per revolution.
FR = {RPM x T x CL}
Where:
FR = the calculated feed rate in inches per minute or mm per minute.
RPM = is the calculated speed for the cutter.
T = Number of teeth on the cutter.
CL = The chip load or feed per tooth. This is the size of chip that each tooth of the cutter takes

you could variate things if need job done faster up to where drivers, machine, rigidity holds, see 2 examples below:




Means as soon as the CL chip load stays the same its Ok.

However its worth noting that is not a good idea pushing the spindle more than 18000RPM if you want to last. The bearings i mean.

I prefer going deeper than faster, when i want to push.

Its worth noting that some materials have "perfect spindle speed". Like aluminum for example -around 8000rpm. Anyways, the above examples from the previous post are all with the relevant "perfect" speed for the material.

2. These numbers also work for engraving /v bits/. However for bits with included angle 45 and 30 degree is better the feedrate to be 25% slower, cause will easily brake tips. Same is for thinner than 1/8 bits or long bits.

3. Bigger shanks are better,less chatter, but more expensive. Use them for precise jobs. Or paid ones. Sometimes i prefer using 10x 1/8 bits 1/8 shank, than 2x 1/8 bits with 1/4 shank, as they cost exactly the same, but 10 bits last longer than 2. Especially on not so sturdy machine. Its a compromise of a kind. Same with the V cutters.

4
V cutters.
60 and 90 degree do all jobs. Dont bother with 30 and 45 degrees as usually they will brake tips and wood chips at that angle.They are only for special purposes. For small stuff i use the 1/8 as they are cheap, for bigger things i use the 1/4 and bigger. . Buy from Drillman1 the spiral ones, as you can use them for engraving and cutting the work piece at the same time. With a bit of sanding later.

5. when you are more confident after cutting some MDF for example, you should check the machine precision and adjust it if needed. Get some pieces of MDF for the test , digital caliper and read the Mach3 manual.
I have my machine in imperial, so bear with me. The principle is the same. When ready, program a 3 inch line /X axis/ . Cut it using a brand 1/8 bit / not chinese- again/ , deep as the diameter. Rapidly measure with the digital caliper. Rapidly, because after a minute or 2 the MDF expands so the measurement will not be correct. Keep the caliper 90 degrees. Now if the line is correct distance, repeat with Y axis. If not, go to the mach 3 screen for the motor step adjustment and make the router move in X 3 inches. When it asks what is the actual distance you measured, fill what you measured. Then repeat until eliminating human error and everything is correct on X and Y. Cut a circle and a square, if they look nice and measure correctly, here you have it. Meanwhile check the suggested steps in the motor tuning dialogue. And hit the save button. And keep a backup of your xml file.

6 About the zeroing
Forget for a moment the touch probes, custom screens,zeroing scripts and so you have seen on the forums.

My everyday zeroing on wood is the following:
-first in Aspire/my CAM/, i almost always use the 0 to be on the top center of the material, not its edge. So its easier to mark using 2 diagonals the center on a square or rectangular piece of wood. Even on circular. Then check with ruler if needed.
-hit the TAB button on mach 3. Set feed-rate to 3. Hit F5 and start the spindle/ if its connected via your breakout board/. Or just start it. So with this slow feedrate using the arrows buttons on the keyboard, move the thing and touch the center. Hit the XYZ buttons to 0. Lift the spindle. Stop it. Now you have zeroed. Simple, isn't it.

Zeroing scripts and touch probe ring/made from copper tube/ i use only for aluminum.