Hello Guest it is June 24, 2019, 10:34:36 AM

Author Topic: Spindle Speed Encoder  (Read 4678 times)

0 Members and 1 Guest are viewing this topic.

Spindle Speed Encoder
« on: November 13, 2010, 07:22:20 PM »
I have a bridgeport R2E3 mill and it has an air driven motor that controls spindle speed so at this point i can't use closed loop feedback to control speed but I bought a cnc4pc index pulse card in hopes of using it to be able to use IPR feeding on the z for more accurate tapping. I'm controlling the machine with mach3 with an ajax cnc motion control card. I tried to hook the cnc4pc index card to pin 15 on my pc parallel port and connect it to mach3 through that access point in ports and pins but even though i've verified 5v and an output htz that moves with spindle speed( using a multi meter ). The onscreen led for inputs doesn't light up. Logically all I can think of is that since I'm using a motion control card that mach3 isn't letting me use the parallel port. HELP!!!! Please!!!

Offline Hood

*
  •  25,846 25,846
  • Carnoustie, Scotland
    • View Profile
Re: Spindle Speed Encoder
« Reply #1 on: November 13, 2010, 07:31:21 PM »
I replied to your PM but afraid I misread it.
You are correct in that the PP is not used when an external motion device is used but does the Ajax not have spare inputs you can use?

Hood
« Last Edit: November 13, 2010, 07:35:13 PM by Hood »

Offline Hood

*
  •  25,846 25,846
  • Carnoustie, Scotland
    • View Profile
Re: Spindle Speed Encoder
« Reply #2 on: November 13, 2010, 07:41:17 PM »
Also I have never used FPR on the mill, it works well on the lathe however so no reason to suspect the Mill would be different. Mach however does not support rigid tapping unless using a servo for spindle then you need to use the swap axis function.
I presume you may well be using a floating holder for tapping though?

One thing to remember that as Mach does not close the loop to the spindle or any other axis motor for that matter (Servo Drives do but not back to Mach) So if you were using FPR it would be read at the start of a move BUT  not during the move so any variance in spindle speed would be ignored with regards to axis motion

Hood.
Re: Spindle Speed Encoder
« Reply #3 on: November 13, 2010, 08:04:21 PM »
Thank You. I was unaware that mach wouldn't update during movement. I thought that in FPR that if it were given a comand to feed at .2 IPR then it would watch the true spindle speed to know how fact or slow to move the z. but knowing that it only looks at the rpm at the start of the thread if it was reading true spindle speed at least it would have an accurate starting point. As it is know I have a very crude dial on the face of the machine that measures rpms by the 50's 100's and 500's depending. I will be threading at around 60 rpm and if the spindle speed dro was working i feel that at that rpm the machine has lots of torque and shouldn't slow more than a couple rpm while cutting so it should be pretty dead on. but as it is now i'm having to program an rpm and then try to make the machine actually turn that fast with my old junky dial. Also the ajax motion control card does have extra io but didn't come with any instructions on how to get those inputs to talk to mach3. And I'm still learning as I go so even though I got the controler installed and working rather quickly that was because they had lots of info and detailed instrutions on that part know I'm working on my own little projects and that's where the funs begining. Haha. Do you think a induction motor with a vfd in conjunction with the index pulse card would help. I know that on tormach's website their duality lathe uses mach 3 and their threading with only an index pulse on the lathe spindle while using the mill table for the lathe x axis and the mill spindle w/rigid mounted tool for the lathe y. I think that this tech is simular to what i'm wanting to do. All that being said I don't have a tormach machine nor do I know how their getting it to work in that manner with mach3.

Offline Hood

*
  •  25,846 25,846
  • Carnoustie, Scotland
    • View Profile
Re: Spindle Speed Encoder
« Reply #4 on: November 14, 2010, 05:48:05 AM »
First thing to say is there is a vast difference between Threading  (single point lathe ) and Tapping.

Threading only requires the Z axis to start at the exact same point (distance and angle) for each pass and the axis to move at the defined feed per rev of the true spindle speed. With lathe threading the actual spindle speed is monitored during a pass and the Z axis speed is adjusted accordingly (within reason).
  However and here is where the big difference is, the tool exits the material at the end of the pass and the spindle does not have to slow, reverse and accelerate, so the axis does not need to be totally in sync with the spindle at all times.
.
Tapping requires the Z axis to move completely in sync with the spindle as it  needs to slow and reverse in sync with the spindle at the end of the thread. Because Mach is a buffered system that is almost impossible to achieve unless as mentioned above you have a Step/Dir motor (servo/stepper) on the spindle acting as an axis. If you had that then the axis (spindle now an axis as well as the others) motion would have been planned taking into account the acceleration etc of each axis and would assume that each axis would keep to that, which they should or it means your motor tuning is no use.

Doing tapping whether on a lathe or a mill can be achieved with good results if you use a floating tap holder, this allows for any slight variance in spindle speed and Z axis feed but more importantly allows for float whilst the spindle and axis slow, reverse and accelerate.

One other thing you may want to look at is Thread Milling, this is easy to achieve on a mill as the spindle speed doesnt come into the equation other than for surface speed of the tool. So in thread milling all you need is for X Y and Z to move in sync which Mach can easily do.

What you mention last is using a mill to thread like a lathe and that is possible and as easy to do as it is on a lathe but I am not sure if G76 threading cycle will work on a mill profile, you may have to open a lathe profile to achieve it.


Hood