New Rebuild on Sherline Chucker Lathe & New build on 5400 mill

[BillB]

A reversible drive will be more expensive.

Run the spindle benchtest to make sure Acorn is outputting the correct analog spindle voltage. You need to isolate where the problem is, Acorn, KBSI-240D, or KBIC

Ok will do.

Did you create a report when everything was working?
Yes

I would create the Wizard Screenshots, rename the CNC12 directory, do a fresh install of CNC12, hand key in all the machine parameters into the fresh install using your screenshots and import your license if you didn't create a backup before tinkering around with macros.


what is "myfun.mac"?
Sorry myfun55,56,57 ect. Was setting them up for XYZ 000, Z0 x0 y0 etc.

[suntravel]

Bill,

myfun55.mac will not make fun, because it will do nothing

The functional name is mfunc55.mac

Uwe

[BillB]

Bill,

myfun55.mac will not make fun, because it will do nothing

The functional name is mfunc55.mac

Uwe

I just got the name wrong when I was posting

Hey for your lathe build is your spindle motor a DC motor? If yes what speed controller board did you use?

[suntravel]

I am using JMC AC servos for my machines to drive the spindles.

Small, powerful and excellent to control.

Uwe

[BillB]

Hey all,

I thought I was out of the woods and home free and ready to finish learning CNC lathe work and start making some parts. However, I have been plagued yet again with many more issues in my lathe build. Please see the video, there are some pretty odd things going on when posting an Intercon file to the control. Please let me know what you guys think. Ive been working on this project nights and week ends for 11 months now and thought I was ready to make my 1st parts so Im very frustrated, so sorry if you can hear it in my video.

IS CNC12 corrupt, is something set up wrong in my settings, OR im I just not doing things correctly yet?



Also includes the Intercon part file

[cncsnw]

I only had time to watch the first three minutes of your video, but a couple things stand out.

Your biggest issue is probably that you are trying to cut at a feedrate of 10 inches per revolution. If you meant to use 10 inches per minute, then you need to go back to the feedrate lines and press F1 to toggle the mode from Feed/Revolution to Feed/Minute. Trying to move 10 inches per revolution, at a significant spindle RPM, is going to result in a feed request (pulse rate) that your drive cannot possibly keep up with. That is why it is losing position with each pass.

Second, you are asking the control to run your spindle at whatever RPM it takes to maintain 2500 surface feet per minute (constant surface speed mode). On a 0.375" diameter, that would require about 25000 RPM. Of course, the control cannot, and will not try, to run the spindle faster than the maximum RPM you have it configured for. The unreasonable surface speed request just means your spindle will run at max RPM all the time.

Third, you have set the end of the stock to be Z0 (per standard practice), but you have then written a program to turn the diameter down between Z0 and Z+0.500. To do anything useful, you will want to make the Ending Z value negative. That error would have been evident on the F8/Graph screen, which you should always check before running a program.

[BillB]

See my comments between and at bottom of yours.

I only had time to watch the first three minutes of your video, but a couple things stand out.

Your biggest issue is probably that you are trying to cut at a feedrate of 10 inches per revolution. If you meant to use 10 inches per minute, then you need to go back to the feedrate lines and press F1 to toggle the mode from Feed/Revolution to Feed/Minute. Trying to move 10 inches per revolution, at a significant spindle RPM, is going to result in a feed request (pulse rate) that your drive cannot possibly keep up with. That is why it is losing position with each pass.

REALLY, So it’s actually loosing steps after the very first pass? Dam never even considered this. WHY dose the cutter never retract and go back to the start of the cut then? Has it already lost its location that much, I will play with these settings and report back.

Second, you are asking the control to run your spindle at whatever RPM it takes to maintain 2500 surface feet per minute (constant surface speed mode). On a 0.375" diameter, that would require about 25000 RPM. Of course, the control cannot, and will not try, to run the spindle faster than the maximum RPM you have it configured for. The unreasonable surface speed request just means your spindle will run at max RPM all the time.

OK

Third, you have set the end of the stock to be Z0 (per standard practice), but you have then written a program to turn the diameter down between Z0 and Z+0.500. To do anything useful, you will want to make the Ending Z value negative. That error would have been evident on the F8/Graph screen, which you should always check before running a program.

Thanks for the input.

As per your input on programming negative Z
Can you watch the rest of the video for me, because the tool move goes the wrong direction (in z +) when I program -.500. I show in the video programming it both with + and - values. Do I have my Z axis set up wrong? Not sure how that would be possible becouse the slide moves the correct direction based on jog buttons.

I figured it would be best to learn right off the bat feed per rev and constant surface speed, it makes sense what your saying, Can you offer the any input on best way to approach learning lathe cnc when it comes to FPM and CSS?

[tblough]

Insert manufacturers have tables for feed per rev and surface speed for various materials. There are also on-line resources such as FSWizard https://app.fswizard.com/, as well as mobile apps and PC apps for calculating speeds and feeds.

Your machine is moving backwards because you are loosing steps by attempting a 10" per rev feedrate. The control thinks it has machined toward the chuck by the length of your part. It then backs up to the length of the part at a slower feedrate where it's not loosing steps so that move is correct. It then proceeds to try and make the next pass at 10"/rev and stalls again, while again successfully retracting the length of the part for the next cut. That is why it is appearing to feed backward!

This is also why it will move past your soft limits becsuse there is no longer any relation to the coordinates you have set. The physical switch is a home switch, not a limit switch the way you have chosen to set your machine up, so it will be ignored once home has been set.

Since Acorn is open loop, once you loose steps for any reason, any settings related to machine position, such as home position, work offsets (X and Y zero positions), soft limits WILL BE WRONG. You have to re-home the machine snd reset your part zeros (unless you are using ZRI) ANYTIME you loose steps.

[suntravel]

......

I figured it would be best to learn right off the bat feed per rev and constant surface speed, it makes sense what your saying, Can you offer the any input on best way to approach learning lathe cnc when it comes to FPM and CSS?

related reading:

https://openoregon.pressbooks.pub/manuf ... -and-feed/

Uwe

[cncsnw]

https://openoregon.pressbooks.pub/manuf ... -and-feed/

That looks like a good reference, but it could use some editing. In several places they say "IPM" when they meant to say "IPR".

A good rule of thumb: if an inch feedrate value is much less than 1.0, it is probably inches per revolution; and if it is more than 1.0, it is probably inches per minute.