EMCO TM 02 Turning Center
To begin the operation of the red Emco turning center here in our lab at Mt. Hood Community college. First step is to turn the main power on. To do that turn the breaker on, followed by the machine power button. The order in which we do this is extremely important because of the power conversions that take place between the European standard that’s inside the machine tool and the American standard on the main power coming in and it goes through some kind of main power converter. Show us the main toggle again. The main toggle is this one the first one that we do followed by the machine power, now we notice that when the machine power goes on the cooling fans for the electrical components for the machine come on you can hear those running. As we come around to the front of the machine we notice that the work light is on on the inside and we notice that the control has begun it’s initialization process. This error message here is telling me that the emergency stop is on so if I turn that off I not have an alarm telling me that the reference position is not set. That means we need to calibrate this machine tool before we do anything else. I press the clear entry button which is CS on the control, I close the door because this machine requires that the door be cycled, I turn the hydraulics on using the auxiliary mechanism. What you just heard is the auxiliary hydraulics coming on. And now I have highlighted this point on the screen the reference indicator telling me I need to reference the machine, notice there is nothing for the x and z axis at this point this machine will not run until it’s referenced. So I next press the cycle start button if you notice in the slides the door has to be closed the first thing you did is move the x axis a little bit now it’s going to defines the x reference position factory preset it puts the x value crt and now it’s found the z position. At this point we are ready to qualify the tools.
One of the differences between the emco turning center is that the program workface coordinates are set within the cnc code for the particular part that you’re making so we do not have to qualify for a particular axis position. What we do qualify for is the tool length. The steps in qualifying for the tool length are:
first off all I’m going to make sure my turret or my chuck is closed and I got a work piece in here.
I next jog my turret to an empty position and I have 3 tools in here so I’m going to come down to a position like that number seven position which gives me an empty turret position. Now using the jog buttons I’m going to move using the manual jog buttons I’m going to use my override switch set a 100% at this point I can go pretty fast. I’m moving the turret I move it out in z so it clears the tail stock my next step is to manually jog it down in x I get the turret down in x now I’m going to bring it closer to the face of the part. One thing I need to watch with this machine is I have to be very careful as I approach the work piece and turn the feed rate that I’m moving the a turret at down because if I hit the face of the part and it’s going too fast I’m going to z axis ? overload and then I have to start all over from power down back to where we are right now. At this point what I wanna do is bring the turret up to the face of the work piece and in order to do that first of all I’m going to pull the control unit around so it gives me access to the controller and access to the work piece at the same time. The other thing I’m going to do is slow the feed rate down I’ve got it set at 2% so the jog rate is going to be very slow now when I bring that in I can watch the numbers upgrade on my crt and tell that it’s moving I moved down to 1% now because I’m getting very close. I now have a slight resistance on the paper between the face of the turret and the face of the work piece what I need to do at this point is record the z axis value that shows up on the screen so I’m going to write that down it’s a z in this instance it’s a z seven point zero zero one four. What I’ve done is recorded the value on this piece of paper because I’m going to need that for qualifying the z axis length on my cutting tools. Now with that done, I manually jog the turret away from the face of the work piece. Once I get the turret away from the work piece I’m going to jog up into the x axis and the reason for doing that is that I need to have a safe index position so that I can index the turret. Now that I’ve cleared the part I can go ahead and press the turret index button and move it so that the number 2 tool which is the next one in the a turret is in the cutting position with that tool in the cutting position with that tool in the cutting position we then qualify the tool for the z axis and the x axis length. My steps in doing this again I’m going to manually jog and jog it so that the cutting tool comes down in the x axis slightly below the outside diameter and then I’m gonna manually jog the z axis slide so it comes in almost to the work piece we slow it way down to 1% and begin jogging it in. then I need to check again with my ? gauge. I have a little bit of resistance on the turret. To qualify this tool this is the number two tool I know that because the turret tells me or the crt tells me that number two is in the cutting position. To qualify this tool I press the shift key the T key and the response I get on the crt is that it has an x and it says automatic tool offsets generate. I’m going to change that to the z and I’m going to enter the value that I wrote down on the piece of paper from the face of the turret. So I put in my seven point zero, zero one four enter I do shift T zero two enter and it has now the controller has recorded the length of that tool from the face of the turret to the tip of the cutting edge it automatically calculated the distance and entered it into the control. To qualify the x axis for this cutting tool my next step is to manual a increase my speed a bit I’m going to manually jog the turret away from the work piece I’m gonna jog up in the x axis so is to clear the outside diameter I now manually jog so the cutting tool is over that outside diameter next I’m gonna slow my feed rate down an begin bringing the cutting tool down to the outside diameter of the work piece. As it comes closer and closer what I wanna do at this point is drop it down to 1% again I use my fancy expensive feeler gauge piece of paper. Once I get the cutting tool so I have resistance on the papers just in the similar manner that we would do for any of the turning centers the procedure to measure the x axis on this machine is to press the shift key the T key the x comes up I’m qualifying the x axis so I go ahead and accept the x and I put in a value of one point zero, zero, zero because the stock of the work piece diameter is one inch diameter I next pressed enter I do a shift T zero two enter and now it is written that value into the control. The skeptical among you may wonder well how does he know it to put in the control if I press the edit key and the shift and the T it opens the tool data register and what I had in there previously is for a tool two was a zero value like you’re seeing for four five seven and eight the one three and five and or six were qualified in a previous session. Tool two now has a length of x two point four seven five four and the z value is negative two point seven nine six eight. Those values represent the distance from the face of the turret to the tip of the tool in the z axis and from the center of the pocket that this holder is in to the tip of the tool in the x axis. The negative sign indicates the direction.