Compensation Type set to control or wear?

[huskermcdoogle]

On 10/11/2017 at 7:02 AM, Rstewart said:

The thing I love most about wear is that its really hard to get a CRC alarm cause you didn't make a correct lead-in move.

I struggle with this even using wear.  I need remedial control parameter training for cutter comp.  I get avoidance vector errors in weird places using G41.2.  Sometimes even when a value of zero is in the register.  Sometimes a value of .001mm works...

I have never looked, but is there any decent documentation on cutter comp out there that describes in laymans terms the different types and the strategies to use them successfully?

One thing that I have done recently is add an if statement that ouputs from the post that checks if I have a negative value in my length wear when I use center comp for ball endmills.  When presetting, we always use end of tool, but to make programming easier for quick head angle changes at the control during setup I like to use center instead of tip.  Anyway, so that it doesn't get forgotten or put in when it isn't needed, my post spits out say:

  For center comp

T7 M6
H7
G359
IF[#_OFSHW[7]GT-6.9375] GOTO9999
G5.1 Q1 R6
G55
G43.4 H7
G0 G90 X-21. Y-11.881 Z100. C-90. B-25. S12000 M3 F5000.
Z32.194
Z9.127

No comp

T8 M6
H8
G359
IF[ABS[#_OFSHW[8]]GT1.0] GOTO9998
(Y APPROACH ON)
(INCREMENTAL)
G5.1 Q1 R7
G55
G43.4 H8

In this case I gave myself +/- 1mm of wiggle room in the value of the the wear ffrom zero.   If it doesn't meet that criteria, it jumps to an alarm at the end of the file.

Now, not to stir the pot or change subject, but how many of you guys use cutter radius comp on a lathe?

[nickbe10]

12 hours ago, huskermcdoogle said:

I struggle with this even using wear.

Cutter comp is like holes, nothing but misery, as my old mentor / foreman said often.

It doesn't happen often but I have come across situations where cc just didn't work and caused machine to alarm. Everything appeared to be fine, end - start points etc.....followed by hours of downtime trying to figure it out.

At that time I was working in one of the last Boeing spares sub-contractors. That was all we did ....spares. 6 parts was a big order, soft set-ups the name of the game. We just couldn't afford to waste time on these unexplained stoppages so we ran on the equivalent of computer comp (we were running an APT system).

When you set up a job you measured your cutters and entered the diameters in the source program and posted. If you needed to make an adjustment you altered the value in the source and reposted, we had totally bullet proof posts. At the end of the job you deleted the G - code file, we never stored them. It was the most "hassle free" machining I ever participated in.

Unfortunately it is totally unsuitable for "production work" as opposed to what was essentially prototyping.

Although we are trying to implement the no stored G - code files ( the only way to control the machinists who think they just have to edit the program their way, for no good reason except personal preference), here the no cutter comp just wouldn't work in our normal "job shop" environment.

So I guess the best thing I can say about cc is that it is an unfortunate necessity in most situations.....although I still only use it on finish cuts.

[JoshC]

It would be nice to see a Poll on what the majority of programmers on here are using, control or wear. I am betting its over 75% of programmers use wear but i could be wrong. Wear is my favorite for a lot of reasons but the biggest is lead in moves, its easy to lead into a .625dia hole with a .5" tool with wear, not quite as easy with control. From my experience Wear is way better but I can understand why some are hesitant to switch when they have a ton of legacy nc files programmed under control or a team of setup guys who are unfamiliar with the differences. To me, it would be worth investing the time and effort in switching the shops mentality on this subject due to how much better it can be for them in years to come.

[gcode]

I'm betting it's 90% wear 10% control

[Flycut]

On 10/10/2017 at 7:54 AM, Henk said:

IMHO he SHOULD order this, using both systems will be a nightmare.

We use both wear and control comp here without issues.

All diameter offsets are controlled by G10 code.

The machinist never has to wonder what way it was programmed or worry about changing the offset.  

[Orvie]

When I 1st learned G-code, I used Control Comp because this is how I was taught.

I wrote my programs by hand in front of the control while reading from the print.

I was also taught that the proper way to use Control Comp was to identify my tools in the program with Programmable Data Setting (G10)

G10 L10 P__ R__

This makes it very easy to use resharpened or alternative tools.

This is back when it was common to write programs in a waterline (top down) fashion.

With todays full depth of cut strategies, I would simply reprogram the part.

I program with wear 100% of the time now.

[Guest]

for those following this..

there has been a poll created if you would like to chime in...

 

Edited October 13, 2017 by Guest

[Grievous]

I don't get what this pool will achieve...but anyway.

What I can tell you is that, all of you who just used Mastercam to program with control comp you are bias. I programed in another software for years and I didn't have ever any issue using control comp. In other parts of the world (especially Europe, I don't know about Asia or Africa or Australia) it is opposite...ppl they are inclined to use control comp.

Mastercam sucks at how its handling control comp. That was the 1st thing I noticed when I start using it 12y ago.

There is a reason that in any controller the offset registry call for tool length, and for TOOL RADIUS(some of them tool Ø depending on settings) to be inputted in the controller so specific functions can be performed...like working with compensation....on tool direction(aka g43) and on tool diameter(aka g41 g42). There is a culture who evolved over the years (more in North America) from the inability of a software (who is the best seller in a specific market), to handle some machine functions. One example...I know that most of you guys know, (when we are talking about how ppl are using tool length compensation), that are still ppl who r working different, by using G52 option..and that what is happening when ppl are using wear comp...they achieve their goal by doing things different..they don't put tool rad in machine ..controller compensate that...or with ppl who r using customized posts where they do 5x by puting their tool length in the program. ...all theese methods are TOTALLY fine, 'cuz you achieving your goal to machine parts.....but by making statements that one way is better then another, without having more experience with another software or controllers it is bias.

Mastercam is just a tool, who should be used to simplify the process of creating codes for a machine equipped with a specific controller. For a controller like Sinumerik, Mastercam it is just scratching the surface...you can access not even 50% from what that controller can do....I'm saying all these to point that you should not judge based by what tool you are using......anyway...  YES...if you are using Mastercam, then you are better by using wear vs control, but not because this is the right way but because that's what your tool(Mastercam) can do better when working with compensation.

[Newbeeee™]

^^^ I've NEVER had a CRC alarm from Mastercam Control comp, because defaults are set to 55% for lead in and arc. Talking Fanucs here.

I've had CRC alarms when I've been switching from Computer (no comp) with a small lead in and arc, copied the operation, changed to Control and posted without changing the lead  in and arc back to 55%... - DOH!

[mike93]

On 10/10/2017 at 9:49 PM, Colin Gilchrist said:

Forgetting the correct entry is an easy way to scrap a part. One useful feature of the machine is that is essentially "adds" both CRC columns together when invoking Cutter Compensation. I used this to my advantage recently in fact.

We have a very old legacy job that is programmed using full CRC. So you must enter the actual cutter radius when setting up the job. No problem, we have a tool pre-setter, so it's not a big deal.

The NC program however was created in a CAM system that we no longer have access to. So all we have to work with is the G-code. I found myself needing to make dozens of tweaks in different places. But I didn't want to have to "move" by editing the G-code.

My solution was to use the Macro programming capability of the Control to my advantage. I added lines of logic to write new values to the Tool Offset Wear Registers for both radius, and length. I was able to switch from .002, to .01, to -.03, to .121, all "on the fly". Since the Wear register gets "added" to the CRC field, I could easily move +- from the periphery of the cutter, or tip of the tool. I even had some passes where I would use a negative offset on 'one side' of a cut, then switch the offset to positive, just before the move to the other side. It worked beautifully. I could take a -.0032 cut on the left, then a +.0128 cut on the right. Sooooo much easier than having to use a G52 coordinate shift for each cut on the part. And, the kicker for me was that I could adjust the part without "reprogramming it", since that was rejected by the customer. I was able to show that my modified program matched the original program path in Vericut, so they approved my method of improving the process.

 

[mike93]

It seems like lately the attempt to improve the process takes more time then the improvement will save, even when its more then 50 percent savings???? is changing the feed rate reprogramming is changing depth of cut reprogramming is changing to a dynamic path reprogramming? most people do not even know what a program is. how would they now if you changed it.

Cutter comp, only  computer or wear. if you forget to put a number in  for cutter comp the part will be scrap end end mill broken off.

[greenxman]

omg not this again!  it will never end.

dumbest argument since cam was invented, i think the admin should add a pin this is a restricted topic forever

the easiest fix is pick one and stick with it. even a one man band has to make a rule and stay with it.

that's enough time wasted

[Leon82]

I worked with a guy who programmed all his endmills .499 ect. He used computer all the time.

He also had a part with two separate programs with the same setup. 3 tools each. The part had a boss that was roughed and a hole was spotted then removed to run the other pieces. Then the second program would drill and tap the hole and finish the boss.

I think he didn't want to touch off more than 3 tools