070301-0830 EST USA

What is your criteria for setting the X value for any of the G5xs on a lathe?

Do you ever use G52 on a lathe, and for what purpose?

Do you want to or do you put the % character in comments?
Do you want to put the paren characters, ( ), inside a comment?

Do you know what the word "monotonic" means?

.

"Monotonic" means that the profile doesn't change directions in X (G71) or Z (G72) after the 1st block of the profile definition. Type I roughing requires a monotonic profile, Type II allows "cavities" in the finish profile.

070303-1227 EST USA

dcoupar:

I use a more general definition for monotonic that I won't mention at this point.

What seems strange to me is that HAAS does not explicitly define monotonic in their on-line lathe manual. This is based on a string search for monotonic in that manual. Monotonic shows up in about 3 places with the assumption that the reader knows its meaning. Non-monotonic also occurs in HAAS error codes on the CNC screen.

I presented the monotonic question because a customer loaded a program in their lathe and received a non-monotonic error message, and they had no concept of what the problem was. Monotonic is not in the HAAS index. A string search in the HAAS on-line manual for any of the following produced the results
nonmonotonic ------- none
non-monotonic ------ two results in notes
non monotonic ------ same two results in notes.
Obviously they could lookup the error code number, but monotonic is not a familiar word to most readers.

I am not suggesting that some other word be used, but rather that HAAS should provide an explicit definition of non-monotonic. I think monotonic is a very appropriate word to use, and a word that more readers should understand.

.

I got Haas' definition from page 53 of the HL-Series Operators Manual dated June 15th, 1966:

"Two types of machining paths are addressed with the G71 command. The first type of path (TYPE I) is when the X_axis of the programmed path does not change direction. This is depicted in Figure 3-4. This type of path is called a monotonic path."

Perhaps they removed this from subsequent publications.

070303-1448 EST USA

dcoupar:

I am at the shop now and our hardcopy of the manual, 2000, does provide some definition on page 168 under G71, also on page 308 under alarms 602, etc. They also use the word monotonous. But nothing in the index.

In our 1996 HL1 manual, serial # 9, page 30 under G71 does say "this type of path is called a monotonic path".

Now I have to recheck the on-line manual with a visual search in these locations.

.

070303-1643 EST USA

It appears that the on-line manual has had any definition of monotonic removed. Also there is no section for alarm numbers.

.

I checked three Haas lathe manuals; 1995 has the explanation dcoupar gives, 2002 has the same explanation but 2006 does not mention monotonic, only TYPE I and TYPE II tool paths. However 2006 does mention monotonic in footnotes the same as the current online manual.

The alarm message 603 in VER 06.12N lathe software gives an explanation of what is meant by monotonic: "603 Non-monotonous PQ Blocks in Z. The path defined by PQ was not monotonic in the Z axis. A monotonic path is one which does not change direction starting from the first motion block."

I agree with gar that it is a technically appropriate word; in math it describes a function that always changes in the same direction, i.e. the first derivative never changes sign (I think?).

But it is a bit obtuse; using TYPE I and II with an explanation is more readily undestandable.

070304-0753 EST USA

Geof:

To elaborate on your definition of monotonic I ask is zero the same sign as +1 or -1?

An internet search found this site
http://answers.yahoo.com/question/index?qid=20070224231242AApdrys
This is an interesting discussion on zero.

In here a little over half way under "elementary algebra" is the following paragraph:

"Zero is neither positive nor negative, neither a prime number nor a composite number, nor is it a unit. If zero is excluded from the rational numbers, the real numbers or the complex numbers, the remaining numbers form an abelian group under multiplication."

With this classification of zero as non-signed, then your definition ("i.e. the first derivative never changes sign") is good but not quite complete. So a small addition produces --- the first derivative is zero or never changes sign.

From www.dictionary.com one of several definitions is:

"monotonic

adjective
1. of a sequence or function; consistently increasing and never decreasing or consistently decreasing and never increasing in value [ant: nonmonotonic]
2. sounded or spoken in a tone unvarying in pitch; "the owl's faint monotonous hooting" [syn: flat]

WordNet® 2.1, © 2005 Princeton University"

I really do not know what was meant by "consistently increasing and never decreasing".

If next we click the Encylopedia tab and go to "Monotonicity in calculus and analysis" there is a paragraph

"The terms non-decreasing and non-increasing avoid any possible confusion with strictly increasing and strictly decreasing, respectively, see also strict."

If you click on strict there is a good definition of strictly.

I agree non-decreasing or non-increasing avoids confusion. Note: "monotonicaly increasing" includes zero, whereas "strictly increasing" excludes zero.


Geof since you have several lathes what values do you have in G54 x for each of these, and related to model number?

.

070304-0753 EST USA

Geof:

To elaborate on your definition of monotonic I ask is zero the same sign as +1 or -1?

I agree non-decreasing or non-increasing avoids confusion.

Note: "monotonicaly increasing" includes zero, whereas "strictly increasing" excludes zero.


Geof since you have several lathes what values do you have in G54 x for each of these, and related to model number?

.

To answer your last question first: Zero; we always leave the work coordinate at zero in X and do all the X offset using the Tool Offset.

Regarding your other points I am a bit puzzled. We are talking about a sequence of numbers; coordinates in the case of a machine, just numbers in the case of solutions to a function. If the sequence is progressively more negative, i.e each successive number is more negative than the preceding one it is monotonic or non-decreasing; it does not matter whether you go through 0. The coordinate sequence X1.0, X0.0, X-1.0 is monotonic; surely it is not the individual sign of the value that matters but whether the relationship between adjacent values is consistent?

070304-1202 EST USA

Geof:

My comment on including zero was relative to your first derivative, not to the function itself. Thus, if y = f(x), then the function is monotonic if dy/dx = d( f(x) )/dx is zero or positive. Alternatively if it is zero or negative.

If zero is without a sign definition, meaning it has no sign, then going from a slope of +1 to a slope of 0 would be a change of sign. When we have a number system where the range is -X thru 0 to +X we have three possibilities for sign negative, none, and positive.

In a digital computer system 0 thru +X will be classified as positive, and less than 0 thru -X as negative where the most significant bit is the sign bit and it is 1 for negative, and the number 0 is all zeros meaning that the most significant bit is zero. In this case 0 does have a sign. Here to include a zero slope with a negative slope for monontonicity would require a separate test for zero condition.

.

070306-1231 EST USA

Geof:

On our SL-20 we have our G5x at -11.5660. This is slightly incorrect now because the turret was crashed and realigned. Basically this value is set to align the centerline of an "ID holder" to the centerline of the spindle.

Thus any drill or other tools that work on the spindle center line will have near zero in their X tool offset. Other tools have an X tool offset that can be looked at and easily judge if the offset is reasonable.

Two of our boring bars are -0.9746, and -0.4835 for their X tool offsets. If we subtract the current error of 0.0134 in G5x, then these would be -0.9880 and -0.4869 .

To us this looks like a logical way to view the system. However, there is nothing wrong with your use of zero for G5x. Within reason you can use whatever you want. How many others use zero for the X value of G5x ?

.

070306-1231 EST USA

Geof:

On our SL-20 we have our G5x at -11.5660. This is slightly incorrect now because the turret was crashed and realigned. Basically this value is set to align the centerline of an "ID holder" to the centerline of the spindle.

Thus any drill or other tools that work on the spindle center line will have near zero in their X tool offset. Other tools have an X tool offset that can be looked at and easily judge if the offset is reasonable.

Two of our boring bars are -0.9746, and -0.4835 for their X tool offsets. If we subtract the current error of 0.0134 in G5x, then these would be -0.9880 and -0.4869 .

To us this looks like a logical way to view the system. However, there is nothing wrong with your use of zero for G5x. Within reason you can use whatever you want. How many others use zero for the X value of G5x ?

.

Your comment "there is nothing wrong with (y)our use of zero for G5x" is much more polite than a consultant I had hired to train my guys years ago. I was told it was wrong and only an @#$%^ would do it that way :), however we still do.

My logic is related to reducing the possibility of errors and I will try to explain.

If you have the centerline coordinate in G5x then all the tool offset values are positive.

When entering tool offset values manually it is possible to enter either a positive number or a negative number.

If the number should be positive and by mistake a negative number is entered then it is possible a situation has been created that could lead to a crash; the tool is going to go closer to the centerline, i.e. workpiece, than intended.

Conversely if the number should be negative, as is the case when G5x is zero, and a positive number is entered by mistake the machine will go further away from the centerline and a crash is not likely. Actually it will alarm because it cannot go positive from machine zero.

My consultant had the grace to apologise when I explained my logic.

070306-1439 EST USA

Geof:

I was not criticizing, just wanted your logic. Thanks.

I like your various responses to threads because they show you have a good understanding of your machines, and a lot of other good background knowledge.

.

070306-1439 EST USA

Geof:

I was not criticizing, just wanted your logic. Thanks.

I like your various responses to threads because they show you have a good understanding of your machines, and a lot of other good background knowledge.

.

I knew you weren't criticizing; I phrased things poorly.