I am blind I guess or I don't under the book
on the Heidenhain TNC310.
I see how and can do peck drilling where the drill
comes all the way out of the part but what i want is
just chip breaking retack .01 then continue
like the G73 on the Dynapath control using the
K word and Q word.

Thanks

If I recall correctly, G83 is a full-retract chip breaker and G73 is a 0.01 retract chip breaker canned cycle.

I'm not familiar with the Heidenhain TNC310, but it should say in the manual if it supports these canned cycles or not. Do you have the manual, and if so, can you tell us what it says about these cycles?

i have read this many times and still don 't
know how to right the code for it

can any one post an example for me of
what this would look like

thanks

Originally posted by fjd
i have read this many times and still don 't
know how to right the code for it

I read it a few times, and it really is a poor translation of something :D

What is all the Q201 to Q212 stuff? From the posts I looked at in Onecnc, the format for Pecking cycle 1 for all the Heidenhain are similar, like this:

CYCL DEF 1.0 PECKING
CYCL DEF 1.1 SET UP (rapid plane)
CYCL DEF 1.2 DEPTH (drill depth)
CYCL DEF 1.3 PECKG
CYCL DEF 1.4 DWELL
CYCL DEF 1.5 F
L X Y FMAX M99

If I knew where the Q2** entered into the picture, I might be able to decipher the message.

HuFlungDung

Now i feel a little better thats the same thing i see and have done with my gibbs.the results= the drill comes all the way out of the hole with the code you post and what I am using.That not what i call chip breaking.

thanks

In that text file, what are the character listed along the left side? There are letters, and carats, two part syllables, mixed in with Q parameters?

How do the variables such as
Q202
translate into this:
CYCL DEF 1.3 PECKG

This text file you copied, is there no sample command line given in the book?

It would seem that the post setup I quoted in the posting above, ignores a couple of variables, Q213, which is the number of chip breaks before a retraction (chipbreak distance is automatically .2mm). Also I am not sure if Q205 is covered. It would appear to be the depth of the first drill increment before pecking begins after the second entry into the hole. Q212 may also not be present: because drilling is in the Z- direction, they call it a decrement, but it would be the total distance of each stage of drilling, which is individually broken by Q213.

How those translate into CYCLE DEF something-or-other, is beyond me.

HuFlungDung
Your right there is no sample in this book.
but I will look some more.
I have only been working with this control a couple of weeks
so I am still trying to understand every thing i don't no

fredj

Dear fjd,

You need to run Universal Drilling Cycle. It works exactly the way you want. The Cycle Type is Cycle 203 in TNC 310 Control.

I can send you the relevant information regarding this Cycle if I have your e-mail ID.

smabhyan ck your PM


your right, is see that in the manual i still don't
understand what the code would look like.

thanks

fjd
take alook at sample in 310 pilot
it may help?
best regards
peter

Thanks peter
i have that page in my manual
I am just not sure what the code should look like

the code will end up beining Q defs

Try
G1z-.2
Z-.19
Z-.4
Z-.39
Repeat
In The Program Or A Sub
It Would Seem To Me That Simply Entering A Number At Whatever Q213 Represents Would Keep The Tool Inside The Part Until That Number Of Pecks Had Been Done.

Ex:
Q201 = -60. (depth Of Hole From Surface Of Part)
Q202 = -15. (peck Inc Distance)
Q203 = 0. (surface Abs Location In Z Hole Is Going Into)
Q204 = 25. (r-plane Inc Distance From Q203)
Q205 = 5. (min Inc. Peck Distance)
Q206 = 1. (cutting Feed Rate)
Q208 = 50. (retract Feed Rate 0=rapid)
O210 = 0 (dwell At R Plane Between Full Retracts)
Q211 = 0 (dwell Time For Dulling Tool At Bottom Of Hole)
Q212 = 5. (amount, Per Peck, To Reduce Peck Distance By Unless Peck Distance Is < Or = To Q205. Ex Peck 1 Is -15. Peck 2 Is 10 3,4,5..... Would Be The Min Set At Q205)
Q213 = 3 (this Is The One You Want It Should Tell The Machine To Peck X Times At The Values Described Before Doing A Full Retract Ex: With The Numbers Above This Should Mean This Cycle Will Drill To Z-15. Break The Chip With An Incremental Move Of Z+.2 Drill To Z-.25 [last Peck Of 15. Plus The Second Peck Which Would Be = To (last Peck - Value In Q212 Of .5) Or (15. - 5.) Or 10.) Then A .2 Chip Break Retract Followed By A Z-.5 Peck Then Do A Retract To R-plane And Then Continue To Do 3 Z-.5 Pecks Followed By 1 Full Retract After Each 3 Chip Break Pecks Until Full Depth Is Reached)

Or In Abs Values It Should Follow This Patern:

Z-15.
Z-14.8
Z-25.
Z-24.8
Z-30.
Z+25.(first Full Retract)
Z-.29.8
Z-35.
Z-34.8
Z-40.
Z-39.8
Z-45.
Z+25.(full Retract)
Z-24.8
Z-50.
Z+25.(out And Done)
Next Hole

To Have It Never Fully Retract Just Increase The Value Set In Q213 To Anything Above The Total Pecks Needed To Drill The Hole Like Say 1000.

Good Luck And I Have No Clue What The Code Looks Like Not Knowing What Q### Represents (ie I, K, D, Q Or Something Completly Different) And Having Never Used That Control, But I Have Used Similuar Canned Cycles With The Same Parameters Needing To Be Set.

Good Luck!!

Thanks charnish

you are correct.
Now what i been working on is getting gibbscam post processor
to generate the code for me. the text file for my post file changed and compiled take a lot of time for a guy that doesn't know what he's doing.
I make an edit, compile then test the post file. and record what the effect
of the edit made on the code for the machine.
so its alot of one step forward and 3 steps back.

thanks
fjd

Yes Gibbs is a wonderful show piece and great if all you do is demo some pre-made pre-planed sales pitch. Also it holds a lot of appeal to those who think they could not grasp the so-called "complexities" of a real cam system or just know nothing about machining. Or for those who just like doing everything twice just to get a close to right tool path. GiBBs and others like it are just too convoluted to me and the posts are unfriendly. Too things to look for when buying cam software are do they want to let you have a demo package or do they want you to wait until they give you a full class. If they don't want to leave a demo it means there system is so convoluted and different from anything on the market that you will be very frustrated trying to do anything with it and anyone you hire to use it will need a LOT of training. The second is can they take a copy of a program you run already and in short order (hour or so should be more then enough) post a program from there system that is at least close in format and correctly coded that matches the format you showed them. If they can’t or wont because (insert excuse hare) move on. I don’t know what you’re making or running but for someone who doesn't know CAD CAM I usually tell them take a look at Featurecam or Bobcad if your running mills. If you want the real thing there is only Mastercam and Surfcam in the arena of real CAD Cams although Surfcam is quickly falling out of that category due to a serious lack of attention to lathes and there seeming to be more concerned with frill then function. If you would like to email me what you have so-far (post text and a copy of what you want the format to look like as well as a list of codes) I will see if I can help point you in the right direction. I have access to GiBBs 6.11 every day and I write posts for people all the time but I will worn you I've never even heard of your machine in my 20+ years in CNC programming. crh23444@hotmail.com

charnish you never heard Heidenhain controls and you been in the busines how long?
Sorry to hear that cause i thought any one thats been doing this for 20 years new the name of every contorl being used today.Do you have ascess to conpost II from gibbs also? Or have you never heard of that also?

Please forgive my ignorance I will go back to my work and leave you to figure things out yourself. You displayed such an ablity in the past as shown in your efforts at that drill cycle. To me the answer was explained in the page from the book you posted as clearly as the insults was written in your reply to my offer of assistance. But, hey you must have read something in your book I didn't to make it so difficult to figure out. Besides what can I know, after all I don't know every control out.

Maybe I should ask a question of you given you're better informed and in touch.

Could you possibly tell me the format for a straight line side milling cut on a 5 axis duel spindle Index lathe? I should mention it is on the sub spindle side using the second turret, program 1 not 2 becase program 2 I have turning the od at that same time. I should not assume you know but I'm sure you do that it's control Index's own. You, knowing all controls, know this know this already; You probably run the other one thats in the united states (Calif. I believe)?

Funny thing I did a 3d mill cut on the 7 axis Star yesterday and it was on the sub spindle side which was easy but, that is a fanuc 16 and I did pause program 1 because running 3 tools caused interference problems during that one cut so I only could have two tools cutting at that point. Funny too is, this kind of reminds me of milling the tooling balls on the Maho 4 axis horizontal mill using about 4 or 5 lines of code with math functions and variables doing all the positioning.. sorry I botherd you with that offer to help and hope you can forgive me even though I don't know everything.....

Thanks in advance fjd hope you can help me out....

P.S. 1982 I started so 20 years was off by a little (I'm in denial about my age.....)

charnish

sorry if i insulted you in any way.


thanks

My comments as far as Gibbs is concerned were directed at Gibbs not the users I could have been a bit more careful in my wording so to all those users of Gibbs who I did not intend to insult I do apologize. I was intending to address the sales people who take advantage of people who are new or unfamiliar with CNC and CAD CAM's. I receive calls all too often from people looking for help because their unable to get the support they need and I was merely attempting (poorly) to empathize with some users frustration. I see it all too often, users who buy something after being promised the support they need only to find there sales person suddenly vanishes. Truly I was not intending to insult the users, I meant just the opposite. I do hope any of you forgive my poor writing skills and my absent brain while writing.

this is what i have chaged the drilling cycle to in my txt file then compiled for my pst file
SeqLab ' CYCL DEF 203 UNIVERSAL DRILLING' EOL
' Q200=' CalcCP2FmSurf# space space space space ';SET-UP CLEARANCE~ ' EOL
' Q201=' CalcZFmSurf# space space space space ';DEPTH ~' EOL
' Q206='fE space space space space space space space space ';FEED RATE FOR PLUNGING~' EOL
' Q202=' ABS# Peck# space space space ' ;PECK AMOUNT~ 'EOL
' Q210='' 00 ' space space space space ' ;DWELL AT TOP~'EOL
' Q203= +0' space space space space space space space space ';SURFACE COORDINATE~'EOL
' Q204=0.2'space space space space space space space space ';2ND SET-UP CLEARANCE~'EOL
' Q212= 0' space space space space space space space space space ';DECREMET~'EOL
' Q213=10' space space space space space space space space space ';NUM OF BREAKS BEFORE CLEANOUT~'EOL
' Q205=0.030 ' space space space space space ';MIN PLUNGING DEPTH~'EOL
' Q211=' Dwell# space space space space space ';DWELL AT DEPTH~' EOL
' Q208=1200 'space space space space space ';RETACTION FEED RATE~' EOL