[Kawgomoo]

Which here is a video i made for you of how i am setting up the machine and going about making my cut. At the end of the video is the G Code i wrote using G90 canned cycle.

Hope the video quality isn't too terrible, had to steal the camera from my son

Let me know what glaring errors you spot!

https://youtu.be/tfwMW4qgHos

[chich2]

Kawgomoo, Great to see you help and make a video but I have to ask the question, why didnt you talk through the process of what your doing? To a newbie theres not much help.

Thank you for your input though and taking the time.

Sent from my GT-N8010 using Tapatalk

[Kawgomoo]

The camera is in an underwater case. I don't think the microphone pics up much more than the sound of it being moved around.

The video wasn't meant to be instructional, as I'm still not sure what the hell I'm doing. lol.

Once i get a bit more comfortable in what i am doing, i intend to make a video out lining how to start the machine, touch off and load a program. Mainly for the benefit of my son, who can't learn anything unless its on a youtube video lol.

I had hoped that someone with more experience than i would critique the video. There are still a few things i am unsure of.

When you go into Offset - WorkShift there is "Shift" and "Measurement" i am still a bit confused as to what these do, exactly. I am only setting the "Z" in "Shift" and leaving the "X" alone. Not doing anything with "Measurement" The screen i am refferring to can be seen at 2:19 in the above video.

I am still not sure where X0 and Z0 are supposed to be. Right now I'm setting the machine up as Z0 is the end of the part away from the chuck and X0 is the part centerline. The operator manual mentions making X0Z0 part center line and chuck face.

Do you at any time program the diameter of the part into the machine, so it nows how big it is? Or does this not matter? The G code simple drives the turret to specific coordinates, and thats that, right? the machine doesnt much know, or care if its cutting air or metal.


Thanks! this place has been a great help. Every answer I've had, one by one I've found the answer to here in one way or another. Hopefully i can get this machine making me some money, soon! Im getting hungry over here lol

[chich2]

This is what I did when I got my Femco Durga 25-E.
Once I had my parameters backed up and the memory batteries changed it was time to put the machine to use. Luckily for me I had a VERY experienced person living close to me who is a master at repairing, operating and programing many types of CNC brands. So to get started;

1. Start with a clean Slate. We deleted all the tool offset / geometry library and wear compensation library. I cant remember how this was done but it is required and you must do it if you want to use the machine under cnc. I explain more on this later.

2. Mount your Tools. I loaded a few tools into the turret. On my machine I have a double disc turret so I mounted my OD (Outside Diameter) turning tools in the front disc and the ID (Inside Diameter) turning tools mounted to the rear Disc. On my machine I left pocket no 1 empty and pocket 21 empty. This is because when running cnc, my machine wont let you call a tool mounted on the rear disk unless the front disk is in position 1 and you cant call a tool mounted on the front disk unless the rear disk in is position 21. This is because of the way my machine channels coolant through the 2 disks to get to the selected tool. From memory I can hold 24 tools. So to leave enough room for any of the rear tools to operate, I leave the front tool pocket no 1 empty. You can see this in these 2 videos.

https://www.youtube.com/watch?v=_ZAWvj7p2k0

And

https://www.youtube.com/watch?v=MrqeI6ISozA

3. Set up the machine. Put a piece of bar in your spindle chuck and clamp it. So at this point the machine control (cnc) doesn't know anything about where the end of the bar is, nor does it know how long the tool is that's currently in the working position because we haven't called a tool. (A lathe tool system is addressed differently to a Mill). A lathe has 1 reference tool, and ALL the other tools are offset against this one tool so someone please correct me if I get this wrong. Some people set their reference tool up in relation to the jaws on the chuck some people set it up to the body of the chuck and some like me set it up to a piece of bar in the spindle. Im REALY rusty on How I did this for my reference tool so someone please pitch in on this reference tool

I think what I did was this:
Use the turret buttons on the front control panel to bring tool the into position 1 (tool 2 in my case). Do not call it via the cnc MDI. The physical machine is in position but the control is still "dumb" to this. I'll explain later.
Turn the selector to Handle and use the MPG Hand wheel to move down close to the material in the chuck positioned so you can take a cut across the face of the bar.
Manually start the spindle.
Using the MPG Hand wheel in X, take a skim cut across the Z face of the bar but do not move Z.
Stop the spindle
Press WORK SHIFT
Press SHIFT INPUT
Press WORK SHIFT These last 3 steps placed the Z Cordinate system at Z zero to make the end of the freshly faced bar Z zero.
Still without moving Z axis off its position go to your Geometry page and scroll to tool 1 and type MZ0.0 and press Input. This means for tool 1 "M" for Measure, "Z" is the Z axis and the 0.0 is the distance from the work shift. You must ALWAYS place a decimal, dot, period what ever you call it in your values. Example 100 would be 100.0 and less than 1 would be 0.05 Must have the dot. (You should see Geometry page input your data against tool 1 for the Z axis)
That will now give your reference tool, (tool 1) a zero offset in relation to the work zero.
Now without moving off Z start the spindle and use the MPG hand wheel to position the tool for a light turning pass along the outside diameter of the bar to clean up the diameter of the bar and take the cut.
Stop the spindle
Without moving the axis off X meaning only move the Z if you have to.
Grab your micrometers and accurately measure the diameter of the bar that you just created. Lets say you measured 1.125 with your micrometers
Still without moving off X axis Go to your geometry page, scroll to tool 1 and type MX1.125 and press Input. This means for tool 1 "M" for Measure "X" of X axis and the 1.125 is the distance the tool was at to create a 1.125 diameter job. (You should see Geometry page input your data against tool 1 for the X axis) Im assuming your using Imperial not metric in this example.
MPG away from the bar.
Go to MDI on your selector
Now we call that tool via the cnc PLUS tell it to include the values from the Geometry page. So type T0101 and press OUTPUT/START
You should see your CYCLE START button flash but the machine wont actually move. Thats because we are already at tool position 1 but the cnc has now loaded the data from the geometry page for tool 1. So T0101 is Call T01 for tool1 and offset it by the data that we just stored for 01. Its good practice to always place the offset for each tool number as the same number as the tool. You could say T0105 Tool 1 and offset data stored in the 05 position of the geometry table but thats just a great way to crash your machine. If its tool 1 go T0101 for tool 2 go T0202 tool 3 T0303
You must always call your tools this way in MDI mode and also in your programs or you'll more than likely crash. If for instance you went T0101 then T02 the machine will end with tool 2 in position but with the offset of tool 1 because you didnt tell it to load tool 2's offset. Pretty clear or is that confusing.

As a test now call tool 1 again in MDI T0101 OUTPUT/START
Move your selector to Handle
Go to your POSITION page so you can see your X and Z cordinates
Use your MPG hand wheel to carefully position your machine to X 0.000 and Z to 0.000 Be carefull if you got it wrong you might drive the tool into the machine or bar. Do this with the spindle running or stopped.
Your tool should line up exactly with the face of the bar and the centre line of the spindle and bar. Now MPG move your tool out to the OD of the bar to the measurement you measured before with your Micrometers and Z zero and you should be at the outside edge of the bar. Note you might have a nose radius on your tool so the tool wont be touching the bar but should line up with it when the axis are traveled. Go slowly as not to crash


Thats all for now. Its midnight here on the East coast of Australia so Im off to bed.
Next post will be how to set the other tools up.
I hope this helps you guys out.

Chich

[Kawgomoo]

Chich, i am going to walk through your steps and mine to see if there are differences.

I know right off the bat, i am not using the ".", for the most part my machine likes for me to give it coords in 5 digit format i.e. 1 inch being 10000, when i input the value, it is adding the "." for me. I have noticed i have to use the period when specifying feedrate.

I ordered a Fanuc operators manual off ebay. I don't think its for my exact right machine, and seems to be written kind of generically. But its for the right "series" of control and seems to be accurate thus far. A lot of it is written in a way i can not plainly understand, as i will admit i am not well educated and have no engineering experience what so ever....Hell, I've never even taken Trig.

I still need to get the cable connected between the lathe and laptop so i can backup my preferences from the machine. I believe i have the cable figured out, but once they are connected and talking. I am unsure of how to proceed.

[chich2]

Kawgomoo,
Yes its very different to your video. Im not sure how the decimals work on your machine. At the start of every program I have a line of codes that sets or re-set how the machine is going to deal with the program its about to run. A line of code in a program is called a "Block" The line I put at the start is called a "Safety Block" My safety block tells the machine to act in a certain way and stay acting that way until told otherwise. So for instance my Safety block will have a "G90" for "Absolute mode" not "G91" for incremental mode. Theres a code that sets metric or imperial measurments. Another one that sets feed per revolution or feed per minute. Another sets Radius mode or Diameter mode. Radius and Diameter mode are detrimental to my previous post about tool set up also. So your decimal issue might have something to do with that or a parameter that needs changing.

As for connecting the machine to a laptop, I can help there too but im a great distance from my machine so cant realy help until im home. I had to make a cable and also change my parameters for it work.

Chich

Sent from my GT-N8010 using Tapatalk

[Kawgomoo]

Yes, i am vaguely aware of the "safety block", but i do not have anyone here to advise me what is wise to put in this line, learning by trial and error on this one I'm afraid.

The "master tool" concept also eludes me. Which tool is the master tool? Is this defined by the order in which you program the tool length offsets?

[Kawgomoo]

Which can you tell me about your cut off tool?

I was looking at getting an Iscar style blade and holder like that, but it seems to me the tool holder covers the cam bolts that would tighten it into place.

What am i missing here? Also, are the tool slots in your turret .750"/19mm? I don't have a split turret like that, just a single 11 tool.

[chich2]

My turret holds 0.750 tools. All my tooling was 20mm so i had to mill the tool holders down so that the tip height was 3/4 which is 19.05mm from the bottom of the tool holder. As can be seen in my thread on post #39 http://www.cnczone.com/forums/genera...97833-cnc.html

As far as the parting tool. Mine is a cheap one from Hare and Forbes machinery house. I always get the thinnest parting tool i can find. I was just lucky this blade type holder was not too tall to cover the clamps. Other single piece ones would fit better but you may have to mill them to the correct centre height too.

Chich

Sent from my GT-I9505 using Tapatalk