DIY CNC Configuration Confusion

Hello everyone,
This is my first post here and I am really hoping something can shine some light on what I am doing wrong.

I built a desktop CNC machine and now I am testing and trying to dial in the machine for accuracy. I created a file that has two 3/8" holes, and when I cut the holes on the CNC machine they are not 3/8" holes they are smaller and not round:confused:. I have adjusted the config changes thinking that maybe my latency is off or my driver settings etc. I cannot get this machine to cut a circle and of accurate size.

I am sure that there is a ton of variables here that could cause the issue to include the overall accuracy of the machine I built, but I hope the information I am providing helps and someone can get me pointed in the right direction to resolve this issue and move forward on this project.

Thanks in advance,

CAD/CAM Software: Vectric Cut2D
CNC Software: LinuxCNC



Stepper Motor:
· Japan Servo Co. LTO
· Type: KH42JM2B086
· DC 5.5V / 1.2A
· Nema-17 Stepper
· 1.8/DEG/STEP
· 200 Steps Rev

Stepper Drivers:
· StepStick A4998 Pololu
· StepTime: 1000
· StepSpace: 1000
· Direction Hold: 200
· DirectionSetup: 200
· Base Period Max Jitter: 24107

LinuxCNC Axis Config Settings:
· Step/rev: 200
· Driver Microstepping: 1.0
· Pulley Teeth: 1.0:1.0
· Leadscrew Pitch: 20.0
· Max Velocity: 0.2
· Max Acceleration: 30

Hi do you have measuring device (like a dial Thing ) Run each axis back and forth and measure if it is precise. You will for sure find an error here like One axis in One direction is limping fix it and here you go ,..


Gesendet von meinem iPad mit Tapatalk

A picture of the machine might help. Pictures of the holes, too.

Small circles can expose even small amounts of flex or weakness and a machine. Circles not being round may also be an indication of backlash.

What speeds are you cutting at? Try cutting at half the speed, at shallow depths of cut, and climb cutting.

My resolution in the config is set to 4000 and if I go to make a larger circle it does look better, so maybe I will look at the backlash on the "Y" axis. I am not able to give you the speed of the spindle because it is a Dremel (20,000 to 30,0000 rpm) and I ran it at maybe 28,000 rpm.
Feed Rate: 15.0 inch/min
Plunge Rate: 10 inch/min

Here are some photos of the machine and the holes that should be 3/8"(.0.3750), but they are measuring at just smaller than 5/16 (0.300).
Attachment 233332Attachment 233334Attachment 233336Attachment 233338

If your cut is a different size than your cad/gcode file, you need to check your motor steps per unit, screw turns per unit calculations. I don't know what hardware or driver software you are using so I can't tell you the correct settings. If you use Mach it has a routine built in to help you set your steps per inch/mm etc.

If your hole is out of round or has flats on one or more sides, you're loosing steps on one or more axis. The cause could be many things... loose motor shaft to screw connection(s), backlash, binding, weak motor (not enough torque), noise/interference in signals to motors, bad wiring connections, loose spindle bearing or mount, out of square axis, and so on. You need to do some reading on the causes and start checking and eliminating until you locate the issue. Many problems can be narrowed down by checking things like, is the error consistent? (same place same amount of error) does is still occur if you swap motors or axis's?, Are you getting excessive backlash when you measure for it?? Is it random or always happens with every cut? And so on... It's impossible for anyone to tell you why your machine is having these issues without a whole lot more information and taking some trouble shooting steps, but with some searching through the forums and reading, you should be able to narrow it down.
Good luck.

dremel spindle flexing?
try using a pen instead of a cutting bit, to see what it looks like

I bet if you push on the collet, it moves quite a bit from the gantry rods flexing. I see a lot of other places for possible flex. Your best bet imo, is too use a much shorter tool, and take very light passes.

Thank you guys for the fast and detailed info. I will work on those suggestions and post my findings.

Sent from my SM-N900T using Tapatalk

Okay, last night I some changes and will post them here when I get home, but my Base Period was off along with changes with the driver step, dir, hold.
I am now getting a better circle when I take .250/path. I get a slightly larger hole if I take .0313/path. I do not understand that, maybe flex?
Any thoughts?

Sent from my SM-N900T using Tapatalk

Quote:

---

Originally Posted by h20frks

Okay, last night I some changes and will post them here when I get home, but my Base Period was off along with changes with the driver step, dir, hold.

---

It is hard to tell from your pictures but it appears that the holes are out of round and significantly so on one side. This makes me wonder about a couple of things. For one do you plunge straight down for each successive cut? Two; you may have mechanical issues.

Quote:

---

I am now getting a better circle when I take .250/path. I get a slightly larger hole if I take .0313/path. I do not understand that, maybe flex?

---

Is that a typo? I don't see how it even possible to put a 1/4" cutter in a Dremel, same thing if you mean a 1/4" deep. Take the diameter of your cutter and go no deeper than half a diameter per pass. That isn't much for a 1/8" Dremel tool but You have to realize the Dremel isn't rigid at all. Once you get the machine set up correctly you can play with more aggressive rates.

As for the slightly large hole with the lighter cuts that would make sense from the reduce load on the tool and thus the reduced deflection. Frankly with a Dremel you are likely to see a difference between climb milling and conventional milling.

Quote:

---

Any thoughts?

Sent from my SM-N900T using Tapatalk

---

Here is a big one, don't go hog wild with parameter changes!!!! When it comes time to make changes keep a log of every single change you make from the default values you started with. It is fairly straight forward math to figure out how many steps per inch you should have, set you machine up first with those calculated values. If the machine is grossly out of whack with those values then you ned to figure out why!! Considering the looks of your machine I'd give the machine a through going over mechanically looking for anything loose and unacceptable backlash.

Again I really appreciate everyone’s input. As you can see from the pictures I am just getting started in building a CNC machine and this is my first experience with everything CNC related. I am having fun learning and I have a long road in front of me.:wave:

A bit of history-
My goal was to start with something simple and low cost in hopes that the machine would be able to mill upgrade parts for a stronger more stable machine.
The machine is very basic and it is using parts that (I am sure is affecting) my results. My thought was if I take shorter passes I would be able to get the results to mill out harder material (wood for now) and then work on upgrading the axis to liner slides and acme screws in hopes for a more accurate machine and be able to upgrade the spindle to a Bosh Cult trim router (maybe I was dreaming).
This leads to me to this current post and you guys helping me to identify issues that I need to resolve. Here is my Mill configuration settings that I am going to mark down as my starting point and will take your advice Wizard and will make small changes and document them so I can keep track of the direction I am going and the results I am getting.

What I was trying to explain in my earlier post about the slightly larger circles is.

I am using a 1/8 4-flute (not 1/4 sorry) end mill and here are the settings I used to get the 3/8 circle

Pass Depth: 0.250
Stepover: 40%
Feed Rate: 60 in/min
Plunge Rate: 30 in/min
Pocket- Raster/conventional with a Profile Pass Last

The settings that gave me a slightly larger circle was
Pass Depth: .0313 in
Stepover: 40%
Feed Rate: 60 in/min
Plunge Rate: 30 in/min
Pocket- Raster/conventional with a Profile Pass Last

I am posting some pictures of the results. The top two circles are with the .0313 per pas depth and the bottom two circles are with the more aggressive depth pass of .250. The rod is a 3/8” rod and it is really tight in the bottom two circles (measuring at .374) and loose in the top two circles (measuring at .380).
Attachment 233556
Attachment 233558

What CAM software are you using? Is it a raster pocket?

Try the shallower depth of cut, but climb cut. Conventional cut will pull the bit into the material, resulting in a larger hole. Climb cut will push the bit away, resulting in a smaller hole. With the flex in your machine, you're going to have find a setting that gives consistent results.

Ger21,
I am using Vectric Cut2D software and the pocket is Raster conventional cut. Thank you for explaining this and I will play with some settings to see what works best for my machine.


Thanks!!

Wow! What a difference in just that small setting change to "climb" and cutting .0625 per pass. I think I am moving in a positive direction thanks! :cheers:
These pictures are showing that I do not have a straight cut does anyone have any suggestions (would even smaller passes improve this)?

Attachment 233606
Attachment 233608

Sent from my SM-N900T using Tapatalk

Quote:

---

Originally Posted by h20frks

Wow! What a difference in just that small setting change to "climb" and cutting .0625 per pass. I think I am moving in a positive direction thanks!

Sent from my SM-N900T using Tapatalk

---

When you have a machine with many sources of deflection and backlash you really need to work to minimize cutter loads. In your case you start right at the spindle which is far less stiff than ideal. If you get the machine cutting with decent accuracy you should be able to then fabricate parts to stiffen up the machine further, Everything from improved Dremel mounting to better slide assemblies with help but here is the big issue you can only accomplish so much with a Dremel and a machine built around unsupported rails. After you get past this learning period you will probably want to build a new machine. It is pretty obvious to me that you have some mechanical deflection in your cuts.

One very important skill to develop is the understanding of feed rates and chip loading and how they affect your results. When you are CNC machining you have little feedback on how the cutter and spindle are handling the load compared to machining by hand. It comes down to what you can hear and possibly an ammeter if you install one. So you have to do some research and some testing to see what you can do for each cutter you intend to use.

In any event looks like you are off to a good start learning CNC machining. Have a happy G-Code day.

You need to make sure the Z axis and/or spindle is perpendicular to the table.