Control vs. Wear

[Guest CNC Apps Guy 1]

Ok, now for my 2¢...

 

Wear is far superior IMNSHO because of all the reasons that were mentioned above and more. I could care less if the numbers on the print match the numbers in a program honestly. If the model is good, and the part was programmed from the model, then the program should be good. Besides programming at the control is most definitely not in the best interests of time with the exception of all but the simplest of programs. You don;t need as much room to get the comp to come in. Les things to worry about. Wear is just better all the way around.

[Thad]

+1 James!

 

Thad

[Psychomill]

Jay, in this case (Mazatrol Tool Data usage), 'reverse wear' won't solve the problem. Mazatrol tool data uses "Actual Diameter" for the tool. Then when a G41/G42 is read, the machine will comp/calculate the radius from that. In mazatrol format, the machine asks for left or right cutting so normal cutting without comp is not an issue. But in EIA/ISO, this could could be a problem when turning comp on/off in the cut. Which is why you "have to" program in 'control, otherwise your tool centerlines will always be a tool radius off.

 

Brian, there is another possible way around this though.

 

If you're going to stick with using Tool Data you can still program in MC using 'wear' by doing this. Now, this is according to the programming book and I haven't actually tried this myself. You can still use a "D" value even though you're using Tool Data. What the machine will (should) do from there is that it will calculate the difference between the tool radius (from Tool Data Actual Diameter) and add/subtract from it the value in the "D" offset. So, with this in mind, you could actually sub-program a set of offsets using G10 for running in the Mazak and still be able to use the same program for the Haas. Just don't read the G10 sub in the Haas. Now, you should be able to program with 'Wear' in MC and still be able to run it in either machine. Just remember to always have 'Wear' on for every toolpath in MC (like you would with 'control'). Other wise you'll have some pretty heavy cuts here and there... But, like I said, I've never actually tried this so I don't know what effect this might have. I would have to change parameters on a machine to use Tool Data to try out this theory.

 

[cadcam]

quote:

---

Jay, in this case (Mazatrol Tool Data usage), 'reverse wear' won't solve the problem. Mazatrol tool data uses "Actual Diameter" for the tool. Then when a G41/G42 is read, the machine will comp/calculate the radius from that. In mazatrol format, the machine asks for left or right cutting so normal cutting without comp is not an issue. But in EIA/ISO, this could could be a problem when turning comp on/off in the cut. Which is why you "have to" program in 'control, otherwise your tool centerlines will always be a tool radius off.

---

I do understand how this works except for the Tool Data as that has been a while for me on that part.

I used to do allot of mold work with High speed Mazaks. But I did not use the Tool data to program with it.

But I know we have this Reverse wear put in into MC just for this issue of not being able to use a Negative Value.

 

I was hoping this would help.

 

Now Can any one tell me waht the advantage to using the Tool Data option compared to say EIA?

[Jack Mitchell]

quote:

---

Now Can any one tell me what the advantage to using the Tool Data option compared to say EIA?

---

Tool Auto Measure (1.2.3.4.5) cycle start and walk away.

Tool Semi Measure (IE: 3" Face Mill)

Diameters are real and easy to use in Mazatrol in particular.

 

The tool measuring is fully or semi automatic. The tool lengths are accurate and any measured tool can be used to establish a G54 "Z". This usually requires that the longest tool be used in an Eia program and that all subsequent tools be measured against such a reference tool as negative numbers. Change a program or change tools for another program then its the same redundant procedure which all takes time and still introduces the opportunity to screw something up. IE: 12 tools equals 12 opportunities to make an error or mistake.

I have run a Mazak using the tool offset page in both centerline comp and contour comp (still nasty cause you need to cut the diameter in half). I now choose to run with the Mazatrol tool data where a G43 H01 grabs the tool length automatically. For contouring & surfacing through Mastercam I prefer to use computer to calculate the path rather than using control for path with comp calcs.

 

Straight up - an operator can set the tools very quickly without the use of calculators & pencils & the opportunity to set a tool offset in the wrong direction = a quick setup with very limited chance for error.

 

One other problem with a Mazak mill is that a G54 will remain constant at power up. Change the value and you will need to shut down and repower the machine otherwise the operator must constantly override the value of "z" for every subsequent tool length measure using feeler gages and calculators.

 

[ 01-04-2006, 03:10 AM: Message edited by: Jack Mitchell ]

[within a thou]

I haven't ran Mazaks but isn;t your G43 subtracted or added to your G54 Z offset to determine your final length?

[beej]

I've learned to give the operators what they want. I got run out on a rail one time when I was younger for butting heads with some operators who were doing some pretty funky old school type things. The boss told me he wanted to bring his shop up to date. But that's not what everyone else wanted I guess.

 

I use wear but if an operator wanted it the other way I'd do it. But you'll have to explain to someone why verifing your program is different.

 

I'm running my own cnc department now and I can't wait for those operators to come back to me looking for a job

[Oppiz]

I have a question...

When using wear how to you keep track of tool size at the control? The tool offset page would only have the minor adjustments in the radius section. seams to me this could get confusing going from program to program, operator to operator. I'm sure the ones the use wear regularly have a good system of keeping this method straight.

[cadcam]

Thanks Jack, Now I remeber using the auto setter and it would pick up the Dia and using the leading tool to set the rest.

I thought it was preaty cool.I dont get much of a chance to run Mazaks any more.

Mostly just program for them.

 

Thanks again

[within a thou]

The way I kep it straight is I always either use wear or computer when programming then the operator can use a set up sheeet and not have to worry about it also I have standardized my tool carousel to number the tool from biggest to smallest using the thinking you will use your biggest tool to rough and smallest for final cuts to help keep it simpilar. When using cam software and with all the indexible tooling out there don;t see why anyone would program off a centerline of a contour. All features with tolerances get wear and all roughing applications just use the computer setting in Mcam

[Psychomill]

quote:

---

Tool Auto Measure (1.2.3.4.5) cycle start and walk away.

Tool Semi Measure (IE: 3" Face Mill)

Diameters are real and easy to use in Mazatrol in particular.

 

The tool measuring is fully or semi automatic. The tool lengths are accurate and any measured tool can be used to establish a G54 "Z". This usually requires that the longest tool be used in an Eia program and that all subsequent tools be measured against such a reference tool as negative numbers.

---

 

Jack/Jay, this isn't totally correct or I'm not understanding what you're getting at here. You can do all of this in EIA offsetting as well and not have to use tool data. Have been for more years than I can count. You can use tool auto measure and semi measure in EIA. You can pick up G54 with any measured tool in EIA and have all positive offsetting. G43 grabs tool lengths in EIA,... even use "tool break checks" in the program automatically in EIA.

 

quote:

---

One other problem with a Mazak mill is that a G54 will remain constant at power up. Change the value and you will need to shut down and repower the machine otherwise the operator must constantly override the value of "z" for every subsequent tool length measure using feeler gages and calculators.

---

Totally lost here..... Never, ever have had to do this... No offense Jack, just not sure about what you're saying...

 

quote:

---

I have a question...

When using wear how to you keep track of tool size at the control?

---

The same way you do now. The "minor" adjustments are just that,... against the cutting size or radius of the tool. In control/centerline programming, you just have the nominal radius already included in the offset value.

[Jack Mitchell]

I did a lesson on comp using Autocad printouts many years ago featuring the comp argument. I would bring the students over to my shop and go through both methods (centerline & contour) and have them fill in the values used. I probably have this lesson on videotape as well but its really tough jamming 20 students around a machine tool while a student tries to capture the information. I will look about for the lesson plan and post it here if I can find it.

This was done on a Mazak using Eia and the tool offsets and might even featuire the same simple program in Mazatrol.

 

Regards, Jack

[Jack Mitchell]

On Jayson's Ftp under the training_files directory.

 

Basic Centerline Mazak.dwg

Basic Contouring Mazak.dwg

These will open with Acad or Mechanical Desktop.

 

The D01 reference actual was D17 since I used the first 16 for length offsets and the next column for radius offsets (the required program edits were also a part of the lesson plan).

 

 

Regards, Jack

[Psychomill]

Interesting.... haven't seen tool length done like that in a long time. Also, by the way you're describing the use of offsets, it sounds like the machine you were using didn't have extended offsetting for tools so you have no 'wear' columns.

 

But even in this instance though, you could still use positive offsetting and eliminate the need for calculating the differences in tool lenths. And/or if you were to use the other "old school" method, and just touched off all of the tools to the part, then G54 could just remain at zero. At that point, if any adjustments were made to G54, all of the tools will still follow without having to figure the differences in tool length.

 

All of this extra work could be eliminated though if you use positive offsetting for tools. Then when the part changes, program changes or the tool changes, theres no figuring that needs to be done at tool offsets.

 

[Andy]

I only use wear comp.

1. I do not need to have the code agree with the print.

2. I like my tool table cutter comp to start out all zeros and change them +- a few .001 as needed.

3. I don't have to enter the different tool dia's into the table every setup and won't make entry errors because all tools are zero dia.

4. As Jim said comping in and out are now shorter distances.

 

However in the days when we used to hand code it was alot earier to go from print to code using on line code with off line comp. (Comp in Control)

[Steel Surgeon]

A little side note from the help menu states-

 

"Do not use compensation in control with remachining operations."

 

 

I am not sure what problem this could cause.

[88Matt]

I must agree that using wear comp is the easiest, safest, and most powerful of the choices in general. But for those who use control comp, have u considered using g10's so the operator doesn't have to input them? Over the next few months I am going to be working on a macro that will pull the data from my tool data and insert it into the NC. This way the programmer (me in this case) doesn't have a typo inputting it either. Any comments, opinions, suggestion, etc. is much appreciated.

[Rick Henrickson The Boeing Co.]

I think Wear is the safest comp to use. If you forget to change D value part is scrap. As far as reading the program shop floor operators shouldn't need to read it and it prevents didlers (people who mess with program just because they feel like it) as far as the Makak and Some Okumas with negative comp, these are parameter settings and you should contact your local machine tool distributor for help If it's an Okuma I can give you the parameter # to change.

[JCLM]

I've always used "wear" but would like to learn more about using "control". A few questions I have about "control".

 

How would you program using a pocket operation?

 

How would you program sweeping surfaces?

 

What about speeds and feeds?

I know that with some of our operators they would be in a lot of trouble if they had to calculate them theirselves.

 

I guess programming with "wear" is the way I learned and unless someone can convince me otherwise, I will probably keep doing it the same way.

 

Jeromey

[88Matt]

Jeromey,

 

There is no reason for u to use control if all your machines will accept wear. The rub lies when u have a machine (like Mazak) that doesn't.

Currently in our shop we don't have this problem (thankfully), but many do. I am starting a little side project that I stated above to insert my g10 code for TLO offline setting. I am doing this for more spindle up time and higher QC. I believe it will also easily do diameter offsets as well, eliminating operators punching at the controls.

 

Please, if I am way off base, save me now before I get started.

[Psychomill]

quote:

---

The rub lies when u have a machine (like Mazak) that doesn't.

---

As I have been saying though, it does. All Mazaks will. It only depends on whether you're using Tool Data or Tool Offset page(s) to pull the info.

 

So 88Matt, you can G10 just about anything relating to the tool. Are you using an external presetter? If so, many of these can be "wired" to the control to upload tool parameters directly without having to create a G10 program.

 

[Jack Mitchell]

Psychomill and I are on the same page - sorry 88Matt

 

 

Regards, Jack

[SaltyAcres]

1)Control is old school, when manually prog were generated yes part surface was better.

 

2) wear is the way to go, if the model is right and the program is right, the oprator should only adjust for cutter dia. differance.

 

3)much safer, if so a 1/2 dia. was on entered,

Bang crash you lose a part for some stupid reason and in todays world of 1 and 2 zee's , you can not afford to take chances

[88Matt]

Thanks for the correction on the Mazak. We don't have any in our shop so I was just going off of others concerns I've heard.

 

I am wanting to standardize several machines of the same model. I will be using a master spindle block on a surface plate for gaging. Using one machine spindle as a master, I am going to adjust the rest through the G53 offset. I can then run the same program with the same tool offsets in multiple machines.

[within a thou]

Matt. I have set something up similar to that but I did it without a master. What I did was set a standard ( I used a edge finder) as say T1. In my height offset page my length offset for T1 is always 0.0 I touch the height of the edge finder where I want my Z to be set using a 2 inch guage block and zero my G54. I then use a 2 inch shift in my machine home co ordinates to comp for my guage block. After thisa is set touch off the remainder of yur tools in your carousel. When you start the next project zero the edge finder the same way and it will update your whole carousel. As long as T1 height never gets changed and is always set in your length offset page as 0.0 no need to touch off tools for every piece. The tools in the rest of the tool pots are the same (T2 is 2' fly T3 1" fly T4 is Cdrill as so on) With a few floater pots in the last spots for specialisd tooling as needed.