[Deco-Doctor]

Hey Martin,
I have an ENC264 and was wondering if there is any way to use my geometry/wear offsets without setting them with a g10? everytime I need to change my part size I have to manually edit my g10. Can I use my g10 for geometry and still use my wear offsets to control part size? Or am I just stuck using g10? Any help would be appreciated. BTW I Don't have a presetter.
thanks
Dan

Hi Dan

The ENC264 is an old machine that I don't know at all, but I will try to help you.

As I understand it you could just alter the wear offset to adjust the size of the part, you could also delete or bracket the G10 comand in the program and then use the geometry offset to adjust the size of the part. I don't think you need to use the G10 to enter the tool geometry as you should be able to enter the tool geometry directly from the control. This procedure is described in Chapter 5.8 of the Manipulation manual.

It is normal practice to adjust the geometry to get the part size correct while you are setting with a new tool, and then use the wear offset to adjust the size of the part while in production.

Hope this helps

Martin

[chetan]

Hi Martin,

What is the use of M90 and M91 command in ENC 162. Actually i have one query that in programm manual they have given sample in which there is no M10 and also no command for returning haedstock. Why is it so?

[Deco-Doctor]

Hi Martin,

What is the use of M90 and M91 command in ENC 162. Actually i have one query that in programm manual they have given sample in which there is no M10 and also no command for returning haedstock. Why is it so?

Hi

Looking at the programming manual the M90 command is 'Reduce speed, fine precise stop'

The M91 command is 'Deviation command, block transition with no drop in speed'

M90 is the default modal command, it means the cutting tool will reduce its velocity at the end of the current block (segment) to make sure the tool makes a momentary exact stop at the end of the block before continuing with the next block. This is to ensure that the programmed cutting tool path is exactly followed.

The M91 command supresses the exact stop of the cutting tool between blocks allowing the cutting tool to make a continuous movement between each programmed block.

The M91 command is used where a cosmetic surface finish is required when an exact stop between segments leaves a visible mark on the surface of the component, for example where there are several intersecting radii along the outside of a part.

When using the M91 to supress the exact stop between segments the tool may deviate very slightly from the programmed tool path.

Hope this helps

Martin

[chetan]

Hi Martin,

Thanks for the help. I m asking you too much about this machine. this is my first cnc m/c. Can you tell me how to use sub routine G160 H9918 (Manual Pg 34)?

My m/c gets stop at G160 H9810. Doest it mean that my m/c has lost this sub routine? If yes then how to get it.

[Deco-Doctor]

Hi Martin,

Thanks for the help. I m asking you too much about this machine. this is my first cnc m/c. Can you tell me how to use sub routine G160 H9918 (Manual Pg 34)?

My m/c gets stop at G160 H9810. Doest it mean that my m/c has lost this sub routine? If yes then how to get it.

Hi

I can't explain to you in a post here how the 09918 subroutine works. You first need to understand quite a bit about the Fanuc Custom Macro programming system.

[chetan]

Actually i need to know that, Do i have to type this program (O9918) and use it at the end of program to change the bar Or it is already available in the control. Does this sub routine depends on the End of Bar Signal.?

I have not yet tried this, but i just want to consult you before practising this.

Infact can you tell me how to load a new bar ( FMB 15 Mini turbo -siemens) without using any Tornos- bechler sub routines ?
Thanks

[chetan]

Hi

I can't explain to you in a post here how the 09918 subroutine works. You first need to understand quite a bit about the Fanuc Custom Macro programming system.

Hi martin

I tried G160 H9902 in MDI mode. The headstock moved forward and crossed it stroke limits giving error of "Over Travel of -Z axis"

and i also tried g160 H9918 inn MDI mode, for this it showed the error "Over travel +Z axis"

Can you tell me why is this happening so? Is there any condition for G160 H9902? How can i load a new bar?

Thanks

[chetan]

What is T column in geometry offsets ? Does it affects the geometry of the part ?

[BauerDef]

Hey, just got our forth Deco last week, 13A. I was writing a program for it, and it generates through fine, but there's a red synchro line between main gang 1 and Z3/X3, what's the deal with that? Doesn't seem to interfere but have never come across this on the 13E or 26A. Thanks

[chetan]

Hi
My machine is tornos bechler enc 162 Fanuc OT. When i use tool for front turning i dont have any problem with diameters. But when i use the same tool for back turning , the first two diameters are coming correctly what i have mentioned in program, but later diameters are coming undersize and some are over sizes. I dont know why is this happening so. The only good news is that every subsequent part is having same variations. I dont know what to do. PLease help me.

[chetan]

Hi,

Can we read the program from EPROM of machine. I tried the parameter 10.4, but it didnt work. Machine is tornos bechler enc162 fanucOT
Thanks

[Ben Odnoral]

Hi
for example,I am running 8.0mm bar stock and threading 61.0mm long a M8 thread using full form tips so on the last cut I want to take about 0.25mm depth of cut- and get the major and pitch dia correct so it doesn't fall out of the guide bush.The G933 threading cycle that runs makes up its own number of cuts and I cant even see what dia it is cutting even in simulation.I tried using G33 cycle but my machine maybe doesn't have that option as it sits there stationary during that cycle and doesn't move the z or x axis.

Have you any thoughts on how to overcome this?

[Deco-Doctor]

I am running 8.0mm bar stock and threading 61.0mm long a M8 thread using full form tips so on the last cut I want to take about 0.25mm depth of cut- and get the major and pitch dia correct

Hello Ben

Cutting a long thread on stock size bar with full form inserts is always a problem on a sliding head. The G933 threading macro will not do what you want here.

To understand why you need to know how the G933 macro is working.

Firstly the macro calculates a Z & X start point for the threading tool and a tool path for the threading tool to follow, ie the X movement inwards, the minus Z movement along the thread, the X movement outwards and then the plus Z return movement to the start point again, a canned cycle if you like.

Secondly the macro calculates an inward movement of the tool from the start point to the final thread depth.

When making the thread the inwards X movement of the tool is superimposed on the tool path canned cycle, this means that the tool is constantly advancing in X at the same time the tool is following the canned cycle path.

The result of this is that the threading tool is actually moving slowly inwards along the length of each cutting pass resulting in a slight taper from front to back of the thread on each pass. The taper is finally cut straight on the last passes of the threading tool with no infeed in X, the 'blind passes' or spring cuts as some folk call them, (G933 parameter 14).

So the number of threading cuts you actually get is derived by the total X infeed distance required to make the full thread and is calculated in the macro as a delay.

You can see the result of this if you put the machine on 'feed hold' during the threading cycle, then only the inwards X movement of the threading tool is halted, the machine will continue to follow the canned cycle tool path, or if you reduce the feed rate over ride during the threading cycle to 50% the number of passes will be doubled for the same reason.

You can see this working in the simulation if you look at the graphic for Z & X and zoom in on the thread, you can also use the cross hairs in the simulation graphic to measure the depth of each pass of the thread, just remember the X measurement is in radius on the graphic.

The G33 threading command is used in exactly the same way, but you have to calculate all the points of the cycle and the delay for yourself (I have an Excel spreadsheet to do this). So the G33 won't help much either! The G33 is not a machine option so the reason it did not work is probably because of a programming error.

Tornos now have a new threading macro 'G978' available as part of the TB-Deco ADV 2009 programming software package. The G978 works more or less in the same way as the Fanuc G76/G78 threading cycle, the tool is positioned at a fixed X diameter for each cut along the length of the thread. So you could do what you want with the G978 threading macro by setting the blind cuts (or spring cuts) to zero so that the last pass of the tool cuts the final thread diameter.

The TB-Deco ADV 2009 software is available from Tornos through your local agent. Purchasing the software provides you with a number of useful upgrades, as well as the new threading macro you will also get constant surface speed (G96) as standard on all your Deco machines.

Hope this helps.

[Ben Odnoral]

Thanks heaps for your information.I will chase up some software.

Hello Ben

Cutting a long thread on stock size bar with full form inserts is always a problem on a sliding head. The G933 threading macro will not do what you want here.

To understand why you need to know how the G933 macro is working.

Firstly the macro calculates a Z & X start point for the threading tool and a tool path for the threading tool to follow, ie the X movement inwards, the minus Z movement along the thread, the X movement outwards and then the plus Z return movement to the start point again, a canned cycle if you like.

Secondly the macro calculates an inward movement of the tool from the start point to the final thread depth.

When making the thread the inwards X movement of the tool is superimposed on the tool path canned cycle, this means that the tool is constantly advancing in X at the same time the tool is following the canned cycle path.

The result of this is that the threading tool is actually moving slowly inwards along the length of each cutting pass resulting in a slight taper from front to back of the thread on each pass. The taper is finally cut straight on the last passes of the threading tool with no infeed in X, the 'blind passes' or spring cuts as some folk call them, (G933 parameter 14).

So the number of threading cuts you actually get is derived by the total X infeed distance required to make the full thread and is calculated in the macro as a delay.

You can see the result of this if you put the machine on 'feed hold' during the threading cycle, then only the inwards X movement of the threading tool is halted, the machine will continue to follow the canned cycle tool path, or if you reduce the feed rate over ride during the threading cycle to 50% the number of passes will be doubled for the same reason.

You can see this working in the simulation if you look at the graphic for Z & X and zoom in on the thread, you can also use the cross hairs in the simulation graphic to measure the depth of each pass of the thread, just remember the X measurement is in radius on the graphic.

The G33 threading command is used in exactly the same way, but you have to calculate all the points of the cycle and the delay for yourself (I have an Excel spreadsheet to do this). So the G33 won't help much either! The G33 is not a machine option so the reason it did not work is probably because of a programming error.

Tornos now have a new threading macro 'G978' available as part of the TB-Deco ADV 2009 programming software package. The G978 works more or less in the same way as the Fanuc G76/G78 threading cycle, the tool is positioned at a fixed X diameter for each cut along the length of the thread. So you could do what you want with the G978 threading macro by setting the blind cuts (or spring cuts) to zero so that the last pass of the tool cuts the final thread diameter.

The TB-Deco ADV 2009 software is available from Tornos through your local agent. Purchasing the software provides you with a number of useful upgrades, as well as the new threading macro you will also get constant surface speed (G96) as standard on all your Deco machines.

Hope this helps.

[chetan]

what does cycle g160 h9809 do in Tornos Bechler Enc162 ?

In programming mannual they said it resets the X axis and z Axis. But is it safe to try this one.

And when do we need to run this cycle?

Thanks

[chetan]

Having problem while indexing spindle in enc 162.
after running M19 command mc shows err "430 : 3rd axis Excessive err". In manual they say " position deviation during stop is greater than setting value." Do i have to set the spindle and pulse coder ratio. If yes what would be its parameter no.

Need help.

[Jfrahm]

Recently bought a this enc-264. I;m in the proccess of getting up and running . Have work through most of it, but trying to figure out how it counts parts and determines end of bar with out telling it how long the bar is, it does not have the presence sensor option. I wrote a macro line to use the fanuc counter to end my program but the machine randomly says its at hte end.
The manual doesn't explain how the subs work, or i think their very cryptic.
Any help would be greatly appreciated.:banana:

[Newby6]

Hello Dr,

I am somewhat new to the world of Swiss turning and have just started programming using the TB-Deco ADV 2009 software. Currently i am programming for a Tornos 20 and 26 and am toying around with the new threading cycle G978. I have been able to use the wizard to write a successful program, however, my cycle time for the operation has tripled to what it would have been had i used the G933. I have tried changing the P15 variable around as well as the blank and empty strokes, but it doesn't seem to help. I am sure i am just missing something or something has been lost in the translation as i am using English Units and have already noticed that variables 21-23 have not been converted to inches. Any help would be appreciated. Thanks in advance.

Kasey

[chetan]

Recently bought a this enc-264. I;m in the proccess of getting up and running . Have work through most of it, but trying to figure out how it counts parts and determines end of bar with out telling it how long the bar is, it does not have the presence sensor option. I wrote a macro line to use the fanuc counter to end my program but the machine randomly says its at hte end.
The manual doesn't explain how the subs work, or i think their very cryptic.
Any help would be greatly appreciated.:banana:

Hi you have to put b4 start of program,
g160 h9810 (deterimnes headstock position and faces off bar)
g160 h9901.
N5 ( block no any you want).
.
.
.
and in the end.
g160 h9902 ( counts the parts and detects the bar has end or not).
G65 h80 p5 ( goes to block no 5).

need any help mail me [email protected]

[mdynas]

I am planning to buy Tornos Bechler ENC 74 - Sliding Head CNC machine - Make 1993 year

Can anyone will provide me its operation manual in english language and the programming method for this machine.

Also please provide me the details about this machine for its milling operation that whether this machine is useful for slotting and face milling operations.

My email id - [email protected]

This Machine is having Fanuc control - OTT - C

Thanks and Kind Regards,

Piyush Patel

Metal Dynamics India