[Deco-Doctor]

Hi everyone

I'm new to this forum, but not new to CNC.

I work for Tornos in the UK and I'm happy to try and help with any Tornos related questions/problems. I look in to this forum most days, but if you need urgent help just send me a PM.

Martin

[hongjianming]

hello Martin

attached file you can find drawing, i don't know how to cut Rectargle threading, pitch; (1.0mm material;titanium)
i worry the tool broken when finishing the threading, could you give me some idles, thank you

[Deco-Doctor]

hello Martin

attached file you can find drawing, i don't know how to cut Rectargle threading, pitch; (1.0mm material;titanium)
i worry the tool broken when finishing the threading, could you give me some idles, thank you

Hi

What machine are you making this part on? If it is the ENC are you using the sub routine O9097?

[hongjianming]

dear Martin
Thanks you to reply very quickly
our plan use deco13a,
you mean this threading can be cut if use g933 code.


thank you

regards

hong

[Deco-Doctor]

dear Martin
Thanks you to reply very quickly
our plan use deco13a,
you mean this threading can be cut if use g933 code.

Hello Hong

Yes you can cut this thread with the G933 macro. The most important point with an internal thread is to make sure you set the G933 parameter P15 (maximum mechanical limit in X) to a small value, 0.5mm for example.

As you have seen already you will break the tool on the return after the first pass of the threading if you don't do this.

To tell the machine that you are making an internal thread the G933 parameter P0 (lead) is set to a minus value, in this case -1.

As the thread has a square form you will also need to set the G933 parameter P5 (threading tool angle) to 0 to ensure the side of the thread is verticle

As an example the following code would work, assuming you have a tool in X1/Y1:

G1 Z1=2.5 X1=7.5 G100
M150
G933 P0=-1 P1=7.8 P2=2 P3=-22.7 P5=0 P6=0.5 P7=90 P8=90 P12=6 P13=1 P14=2 P15=0.5 P16=0.5
G1 Z1=2.5 G100
G1 X1=40 G100
M151

You may need to adjust the P12 value (number of rough cuts) to suit.

Generate the program and then check the tool path for the threading cycle in the SimDeco program, from the menu select 'Graphic' then 'Position' then select the two axes to plot, X1 & Z1. Use the magnifier to zoom to the threading path and check the path looks correct. Use can use the left mouse button click and measure the thread depth with the cursor, the X1 value on the graph given by the cursor is in radius though!

Hope this helps you, good luck.

Martin

[hongjianming]

dear Martin

thank your support

i am worry that the part have vibration if cutting threading,because the threading is square. the material is titanium.

did you cut this kind of thread before? i think the spindle is very slow.

i want to use ID thread whirling, what do you think?

but i don't know how many teeth of tool make?

do you give me some suggestion?

thank you

best regards

hong

[chetan]

Hi deco doc.

We have bought the Tornos Bechler ENC 162. Well i need help regarding the tornos bechler cycles used in this machine. We also have robobar FMB 15 which does not works in auto mode. If you could give us the programming manual or information for this machine we will be very please to you.

We need to know how this tornos bechler cycle works e.g. G160 H9810..G163...G164....G161.... G16o H9xxx TB cycles.... Variables used A..B..C..F..etc. what are this.

And also we are not able to use program test. showing error
"Forbidden prg tst : end of bar "
Please help us in this matter

Thanks in Advance

[Deco-Doctor]

Hi deco doc.

We have bought the Tornos Bechler ENC 162. Well i need help regarding the tornos bechler cycles used in this machine. We also have robobar FMB 15 which does not works in auto mode. If you could give us the programming manual or information for this machine we will be very please to you.

Hello Chetan

I have sent you a private mail.

Regards

Martin

[chetan]

Hello Deco doc

I have sent you my email ID to your PM
Please check it.

Thanks and Regards

[chetan]

Hi deco doc

Is there any limit for threading length in ENC 162?. And can we use two tools at a time, one for rough cut and another for finish?. Actually, bar stock is 14.2mm and i want to use two tools at a time, instead of giving whole load on single tool.

My another problem is, when I set geometry offset in W place for T6, i have to also adjust for other tools and this is messing up the dimensions of part. And i m not able to adjust the distance of part in the mid of tolerance and total lenght also is not coming to that value what i have mentioned in program. Overall We are not getting the distance on part what we have programmed. If you have solution for it please reply me.

Thanks

[Deco-Doctor]

Hi deco doc

Is there any limit for threading length in ENC 162?. And can we use two tools at a time, one for rough cut and another for finish?. Actually, bar stock is 14.2mm and i want to use two tools at a time, instead of giving whole load on single tool.
Thanks

Hi Chetan

You did not say what length of thread you want to make, I assume you mean to screwcut? Normally for screwcutting you dont want to exceed the internal land length of the guide bush, otherwise when the threading tool cuts the bar diameter with a full form insert there will no longer be any support at the bar diameter from the guide bush. You can set the tool further away from the guide bush to increase the length a little, I use a left handed tool for this.

You can use two tools to cut at once, but only for turning, not threading.

Martin

[chetan]

Hi deco doc,

I have PMd you my another email ID
Please check it.

Thanks

[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

[slidingheadfred]

Hi, Martin this may be too much to ask but i have been setting/programing a deco lathe and would like to know if you have any c axis programing examples, as i would like to know about programing this axis, never had to use it so far but would like to know how to for the future.

Cheers.:cheers:
Fred

[Deco-Doctor]

Hi, Martin this may be too much to ask but i have been setting/programing a deco lathe and would like to know if you have any c axis programing examples, as i would like to know about programing this axis, never had to use it so far but would like to know how to for the future.
Fred

Hi Fred

Send me a PM and we can talk.

Martin

[hongjianming]

Hi, Martin this may be too much to ask but i have been setting/programing a deco lathe and would like to know if you have any c axis programing examples, as i would like to know about programing this axis, never had to use it so far but would like to know how to for the future.

Cheers.:cheers:
Fred

hi
you can read in tb-deco software's help menu, the code is m198.

regards

[EvansMachine]

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

[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