[kevinkoons]

Hello Everyone,

We have just acquired an Hyundai SPT-V30 Machining center with a 14 position ATC. This machine was made in 1998 and is in very good condition. We received it in last week on Friday and over the weekend I connected power and air.

I have no user manuals for this machine. While I am not completely new to CNC mills, this particular machine is new new to me and the ATC is new to me.


I am not at all familiar with installing tools into the ATC or into the spindle without the use of the ATC (if that is an option). There are some instructions on the machine in broken English that hint about moving the spindle to the tool change position in order to install a tool holder into the ATC. No idea how to do that. In MDI I am able to execute a tool change (M6 T5 and the magazine works fine, Z goes up and mag rotates then Z comes down to load the tool, if there was a tool to load!

My question is how do I position the Z in the "tool change position"? Simply bringing the Z up will trip an over travel.


Anyone using one of these machines? Any advise on loading tools into the ATC?

Any idea where to purchase a user manual?


Thanks,

Kevin

[JDenyer232]

Not familiar with your specific machine, but I'll try to help anyway. Is this an umbrella style tool changer? Anyway, your tool change position is usually the machines zero position, G28 X0.0Y0.0Z0.0 will move all three axis's to the machine zero position for a tool change. Be very careful using G28 with all three axix's referenced on the same line, if there are fixture clamps or if your at the bottom of a pocket all three axis's will move at the same time, usually causing a crash or at the least breaking a tool. Here is an example of how I would do it.
G00Z1.0 (MOVES TOOL 1" ABOVE PART)
G28 X0.0Y0.0Z0.0 (PERFORMS MACHINE ZERO RETURN ON ALL AXIS'S)
G80G49G94M01 (SAFETY LINE, IE CANCEL CODES)
M5 (SPINDLE OFF)
G00G40G49G80G90 (SAFETY LINE FOR NEW TOOL)
T3M6 (CHANGE TOOL)
S5000M03 (SPINDLE SPEED AND DIRECTION)
ETC.





The 1" above the part is a good safe distance, you would need to go higher if you have clamps that stick up higher than that 1". Is your tool carousel mounted at the front of the spindle? If so you probably dont need to use G28 instead you would do something like this with G53.
(.500 ROUGHMILL)N3G00G40G49G80G90
T3M6
S5000M03
G54X0.0Y0.0
G43H03Z1.0
M08
D03
G1060T0.2D.500S0.05L0.075J0.2K0.015H0.F30.V30.E15. M100.W2.C0.1P3.R0.1Q3.X0.1Z2. (FANUC'S CONVERSATIONAL LANGUAGE)
G1220T2.B0.L-0.2H0.375V0.2U0.75W0.4R0. (FANUC'S CONVERATIONAL LANGUAGE)
G00Z1.0M09 (G00Z1.0 NOT NEEDED, I JUST USE IT FOR ADDED SAFETY)
G53Z0.0 (MOVES Z AXIS TO MACHINE ZERO FOR TOOL CHANGE)
G80G49G94M01
M5
(.625 FINISHMILL)N4G00G40G49G80G90
T4M6
S5000M03
G54X0.0Y0.0
G43H04Z1.0
M08
D04
G1062S0.015D.625K0.B1.F40.V40.E20.W2.C0.1P3.R0.1Q3 .X0.1Z2.
G1220T2.B0.L-0.2H0.375V0.2U0.75W0.4R0.
G00Z1.0M09
G53Z0.0
G80G49G94M01
M5
The G53Z0.0 returns the z axis to the machine zero posistion for a tool change, some tool changers don't need the X or Y axis to be in a certain position. This is true on some of the smaller machines that have the magazine at the front of the spindle. A photo of your machine showing the location and type of tool changer may be helpful.
Use any info provided here carefully, it is only a guide to give you an idea of how it may be done, machines do differ from different makers. Ideally you should order the manuals from Hyundai, it's money well spent when it comes to safe operation and maintenance. Below is an example of a tool changer at the front of the spindle that the G53 method is likely to work for. Hope this is of some help to ya.

[kevinkoons]

Thanks JD for your reply!

When our machine arrived I had no user manual for it so learning things specific to this machine was a little tricky. This past week I was able to order a user manual from a Hyundai dealer and should have it this week.

I was also very successful in learning to program the machine. I was having a difficult time learning on this machine how to establish my work coordinate offsets. I stumbled on to a screen where they are stored and some how deduced the WR key pressed after entering the new position information would update the offset!


I have used machines with Fanuc controllers so this was not all new, just some things particular to this Yaznac MX-3 controller.

My big problem with the tool changer was that with the machine in the home position (X, Y, Z at machine zero) you are not able to snap a tool holder into the ATC at the position directly under the spindle. I know there has to be a command to bring the spindle up clear of the tool changer. I am able to load tools now so not a huge deal, hopefully the manual when it gets here will shed some light on that. The ATC is really nice!! Understand that I had been working with a Bridgeport Series one which I had retrofitted with Mach 3. The Bridgeport is a good machine and Mach 3 is great but this VMC with a fairly modern (1998) industrial control is just wonderful!

Some additional tool holders I ordered have arrived along with some machinable wax so this week I will be learning the ins and outs of rigid tapping, something I was not able to do with the Bridgeport.

[JDenyer232]

Thanks JD for your reply!

When our machine arrived I had no user manual for it so learning things specific to this machine was a little tricky. This past week I was able to order a user manual from a Hyundai dealer and should have it this week.

I was also very successful in learning to program the machine. I was having a difficult time learning on this machine how to establish my work coordinate offsets. I stumbled on to a screen where they are stored and some how deduced the WR key pressed after entering the new position information would update the offset!


I have used machines with Fanuc controllers so this was not all new, just some things particular to this Yaznac MX-3 controller.

My big problem with the tool changer was that with the machine in the home position (X, Y, Z at machine zero) you are not able to snap a tool holder into the ATC at the position directly under the spindle. I know there has to be a command to bring the spindle up clear of the tool changer. I am able to load tools now so not a huge deal, hopefully the manual when it gets here will shed some light on that. The ATC is really nice!! Understand that I had been working with a Bridgeport Series one which I had retrofitted with Mach 3. The Bridgeport is a good machine and Mach 3 is great but this VMC with a fairly modern (1998) industrial control is just wonderful!

Some additional tool holders I ordered have arrived along with some machinable wax so this week I will be learning the ins and outs of rigid tapping, something I was not able to do with the Bridgeport.

Ok, realy quick, there is usually a notch at the 3 or 4 oclock position, this notch is usually on the back plate of the atc magazine, you just count the number of places you need to move a tool to that position. Say you need to index it 3 places to move tool #4 into position. You then enter P3M6; in mdi mode, press cycle start and the magazine will move 3 places clockwise. Load your tool, and you can do the same for the other tools. T will put the selected tool in the spindle, and P will index the tool changer for loading. Hope this helps.

[kevinkoons]

Thanks JD!! This is what I was looking for, will give it a try in the morning!

Everything else is going well and actually started cutting some machinable wax today.

Kevin

[kevinkoons]

The manual for our machine arrived today! I would have been more excited had it been for our specific machine!! The manual they sent was for a similar machine so I was able to figure out how to set the spindle to the tool change position.

On this machine the Px M6 command is not the answer. To get the spindle to the tool change position you have to do so in MDI with a sequence of codes.

G22 Z138.2;
G91 G30 Z0.;

This puts the spindle up to a pre-assigned location (G22) that will allow the magazine to turn using the rotate magazine button when in JOG mode.

With the spindle up you can rotate the magazine and then install a tool holder easily in the bottom location horizontally. Prior to knowing this I was reaching up to either side and installing the tool holder, a bit awkward and sometimes not easy to see that the tool holder was properly seated. Once the tool holder is in position you simply bring the spindle down and it automatically loads the tool positioned beneath it. Pretty simple now that I know! I wrote a short program just for positioning the spindle to the tool change position.


About the manuals, the dealer I ordered it from contacted the factory and they are sending out the proper manual(s). Would you believe we paid $200 for a 33 page .PDF file on a CD? WOW! I was expecting MANUALS as in all manuals for that price. Hope this gets resolved.

Thanks for the replies!

[kevinkoons]

We finally received the manual for our Hyundai VMC! I have to tell you, the manuals for this machine leave A LOT to be desired! One thing I was able to get out of it that was a huge help, according to this manual the control is a Yasnac J50M NOT the Yasnac MX3 as reported by the seller. The machine has no markings on the control as to model or manufacturer. Anyway a quick search of the Internet and there it is, 298 pages of detailed information on the J50M control!!!

Rigid Tapping is now a breeze! Prior attempts were not very successful because I was not able to turn on the rigid tapping feature before calling the tap cycle. Now that I have discovered the M codes (G93 - on, G94 - off) and how to call them everything works perfect!

This is what works on the Hyundai SPT-V30T(D) when tapping 32 threads per inch (in this case a #6-32)

...
G93 S1200.
G84 G98 Z-0.400 R0.200 F0.03125
X3.250
X5.250
G80
G94
....

Spindle start and stop is controlled by the G93 Rigid tapping function and the feed is IPR so the F is set to the thread pitch.

I used a forming tap and spot drilled before peck drilling a .125" x .550" deep hole. I tapped .400" deep. The tap was in a TG100 collet holder, rigid.

Thanks again to all the responded!