anyone familiar with q parameter programming on tnc series that can explain the basics to me? any help very much appreciated.
anyone familiar with q parameter programming on tnc series that can explain the basics to me? any help very much appreciated.
Which TNC
tnc 410
not a lot to them really, if say you were machining an oblong profile and you needed several different lengths you could programme the length into Q1= (length)
then in your programme instead of a numerical value for your "X" move you substitute Q1
eg LX Q1 R0 F0 M. You can also do calculations within a move, LX (Q1+10.0) Y0.0 Also available are all the usual maths functions. the uses these can be put to are limited only by your own ability at maths. I have produced general purpose programmes which can generate corner rads on blocks, angle faces, block up etc. I have programmed a sphere with a 6 line programme using advanced methods. if you look on page 273 of the manual you will find a programme for a sphere but it takes 51 lines. so it is well worth learning. some basic algebra and trig. If you have any specific questions Ill be happy to help you.
Stu.
If you still need help with Heidenhain Q parameters, I sell Heidenhain Basic and Advanced programming courses on ebay. The Basic course has a few programs that use Q parameters. The advanced course has a lot more. There are 84 programming examples altogether, all written by Heidenhain. Just search for 'Heidenhain' or 'CNC Programming' on ebay.
What do you think of the TNC 360 controller - I might have an opportunity to buy a Tos CNC F2V. The owner was using GibbsCam.
Any thoughts appreciated
Karlis
Melbourne Australia
first of all thanks for the help stu, i will contact you if i run into difficulties.
now to answer your question karlis, im not familiar with the 360 but if somebody compares it to the 410 (which i use) i would consider it a good thing. i have lots of cycles and options which make this control very user friendly and i find myself using cad programming only for complex stuff, everything else i program at the machine,
Did you buy it already? It's kind of all right,allowed rigid tapping, for simple milling job it's very good,how do you intend to programm it G codes or heidenhain conversational?,my advice would be,always use Heiden in conversational mode,much easier...
Well basically the q parameters are used as variables, for instance instead of a L X0 to L X5 you would simply define q values such as Q1=0 and Q2=5 and substitute the X moves to L XQ1 to L XQ2. Another thing useful use for Q variables is by programming some logic into the program.
Such as:
When doing contouring with Depths of Cut one can, instead of programming absolute Z movements you could.
Q1=.005 ;Depth
Q2=.001 ;Depth of Cut
Q3=Q1 ;Counter
LBL 1 ;Sets Label
IZ-Q2 ;Steps down in Depth of Cut Incremental
Call pgm Contour ;Contouring program
Q3-Q2 ;Subtracts Depth of Cut from Depth
If Q3 greater than Q2 go to LBL 1 ;queries
IZ-Q3 ;finishes remaing leftover material if any
Call pgm Contour
LBL 0
So with just a few lines of code one can have the program think for itself.
Hope this helps