Control Vs. Wear

[SpecialtyTool]

Can someone explain the difference between control and wear for cutter comp applications? Im using this with a Mazak mill if that makes a difference. I know before when I ran Haas machines we put "0" in the tool data in the machine but all the machinist here want the actual tool diameter in the offset page. I know wear and control will dictate how this is done. Im asking because it seams to generate different tool paths when I switch from control to wear. Everything looks good as with wear but when I switch it to contol and regenerate my tool path the lead in and out change. Im having trouble adjusting it to keep from hitting the side of my pocket as the cutter enters and exits the cut.

 

Thanks

[Guest]

If you HAVE to use control, set your lead in/lead out to perpendicular and a minimum of 50%

 

Wear calculates 1/2 the tool diameter into the path and gives a G41/G42 for adjustment, comp setting generally start at .000

 

Control Comp does not factor in the tool size when it calculates but it gives a G41/G42 for adjustment, comp setting is generally set to 1/2 the dia of the tool.

 

The Mazak using the tool table will likely use the tool diameter.

[Mgrenier]

Wear outputs the center of the cutter and compensate from there. Control outputs the part and the machine compensates for the tool radius. For your leadin/leadout to work in control comp, the length of the move needs to be bigger that the radius of the tool in mastercam. Keep in mind that the radius of the tool will be conpensated for.

 

HTH

 

 

[Rocketmachinist]

Im having trouble adjusting it to keep from hitting the side of my pocket as the cutter enters and exits the cut.

 

That is one of the nice things about using wear vs control. Because you can have a zero value in your offsets you can have cutter comp turned on in a hole with very little room for your cutter vs control where you have to have a large lead in room for your cutter. Stick with wear, nearly everybody on this site swears by it and most of them say they would almost never go back to control.

[SpecialtyTool]

That is one of the nice things about using wear vs control. Because you can have a zero value in your offsets you can have cutter comp turned on in a hole with very little room for your cutter vs control where you have to have a large lead in room for your cutter. Stick with wear, nearly everybody on this site swears by it and most of them say they would almost never go back to control.

 

Thank you. Im used to using wear on a Haas and I liked it but Im at a new shop where they only have Mazaks and just now bought mastercam. All of the machinist are used to using Mazatrol and seeing the actual diameter in the tool data page.

[Teh Bear without Brains kinda idiot]

Because you can have a zero value in your offsets you can have cutter comp turned on in a hole with very little room for your cutter vs control where you have to have a large lead in room for your cutter. Stick with wear, nearly everybody on this site swears by it and most of them say they would almost never go back to control.

~~~~~~~~~~~~~~~~~~~~~~~~~

Not true at all

I always used control and use it now

 

You can have same lead as in wear

What the difference if you have size of leave in 0.01 mm instead of 0 ?

every method has a lot of pros and contras.

[Guest CNC Apps Guy 1]

I'd NEVER go back to control either. Too much of a PITA.

[Teh Bear without Brains kinda idiot]

Let`s say you in production using grinded tools

Your offset anyway is not zero !

using tool with offset +.1 you scrap your inner radius

ETC

And editing toolpath by hand is pain in the *ss

[gcode]

Control comp can be OK if you have a through understanding of the machine and control..

 

but if you're writing code for a big company with numerous machines and operators it is best to stay

 

away from it.

[Aeroguy]

I know before when I ran Haas machines we put "0" in the tool data in the machine but all the machinist here want the actual tool diameter in the offset page.

 

Well my suggestion is to tell your set-up guys to suck it up and live with wear compensation. It's alot easier for everyone anyways to use wear.

[kh012]

don't know if it still will do it but with control comp it used to ignor the look ahead on some tool paths and try

and fit a larger tool into ares that it wouldn't fit. like tying roll a 1/2 em into a 3/8 wide slot.

with wear comp. you don't have that problem. its been awhile since using contol so im not sure if the newer mc's

still do this

 

Ken

[AshM]

I subscribe to using control compensation....

 

Maybe the biggest reason I have never switched is because for in machine tool measuring for length the R value is used to move the tool sideways for length measurement.

 

But one some controllers the added benefit of wear is that you can get errors when you are compensating inside of tight corners and the controller determines the tool wont fit inside the programmed path. When you are only compensating 0.01 mm or so this is way less likely to be a problem. I've only used wear once to get around this, and switched it back straight after the job to avoid angry confused looks from my workmates....

 

Personal choice I guess.

[PeterM]

When I started programming conrtol comp was all that I knew, and you can make almost any tool run without error using it, just follow the rules. I switched over to wear in V9, it is much more flexible, and you generally don't get the big crashes like you might get when the setup guy forgets to input the rad of the new tool and a larger tool was in that tool pocket in the last job. The biggest problem with wear vs control ccomp is with the operators. If you have a large library of old jobs, as we have where I work, then you need to identify which jobs are using what ccomp, or you can expect crashes. I modded my posts a long time ago to state which tool comp is being used, it is part of my setup sheet, and I edit old programs to include the ccomp. We still get an ocasional crash with old jobs.

[gcode]

When I first started programming machine tools, I did it by hand and used control comp.

I switched to wear with my first cad/cam system and have used wear comp ever since.

In the following 20 years, I've never worked anywhere that uses control comp.

It was expressly forbiden in the last 3 places I've worked.

 

In a small shop where you have tight control over proceedures I don't see anything wrong with it,

but in a big shop with 20 to 30 operators of varying experinece levels and multiple models/brands

of controls, using control comp is going to cause big problems IMO

[Mick]

I've never used Wear, only Control (and I hate using control, only using it when I can).

 

However, after reading this thread, I'm going to try out wear. It makes a lot of sense!

 

By the way, how does Reverse Wear work?

[Newbeeee™]

... the big crashes like you might get when the setup guy forgets to input the rad of the new tool and a larger tool was in that tool pocket in the last job.

You could get mastercam to output a G10 line with the related R value which automatically puts the correct data into the control.

[Colin Gilchrist]

I've never used Wear, only Control (and I hate using control, only using it when I can).

 

However, after reading this thread, I'm going to try out wear. It makes a lot of sense!

 

By the way, how does Reverse Wear work?

 

Reverse Wear works exactly the same way as normal Wear, except the Cutter Compensation codes are reversed. So instead of G41 (Cutter comp left), you would get a G42 (Cutter comp right). Some controls require this type of Wear offset (although I've never worked on a machine that does).

[Simtech]

Here's one way to use Reverse Wear in a production shop with many operators ...

 

When we are cutting external contours in climb milling (CW), we use normal wear comp, ie, G41 (left side comp) output. This has the effect that if you want to INCREASE the size of whats being machined, you add a "+" value in the comp of the tool, if you want to REDUCE the size of whats being machined, you enter a "-" value in the comp of the tool. For example, +0.002 will increase the overall wall size by 0.002"

 

When cutting an internal pocket finish pass, in climb milling, we will cut CCW, but at the same time, we will use a G42 (right side comp). This has the same effect then before, ie, that if you want to INCREASE the size of whats being machined, you add a "+" value in the comp of the tool, if you want to REDUCE the size of whats being machined, you enter a "-" value in the comp of the tool.

 

This method makes it a lot easier for the operator to determine the correct "sign" of the comp required to adjust machining.

 

Just my 2%

[BBprecise]

We've always used control here and I've been here for 17 of the 19 years they've had a CNC machine. The shop where the owner worked used control at the time and just carried it over when he started his own shop. The biggest benefit of using control (which I prefer as an operator) is the ability to see print numbers in the program and don't have to compensate for half the tool. Granted a lot of that depends on the zero position of prg and how the part is drawn. New machinists get training on this when they come through the door so no unexpected surprises. Neither style eliminates problems like the operator putting a bigger e.m. or forgetting to adjust the offset when a bigger dia tool is swapped in (only happens with regrinds which we live by). Plus changing hundreds of prgs as they are run would be a nightmare, the only thing I do differently now than we used to is I program to leave stock on, instead of relying on the operator to add to the CDC. This also allows me to see if I forgot to finish something when I use verify. Odd geometries sometimes require turning off look ahead, or messing with the optimize and roll cutter around corners options to get the right path, but that don't happen very often.

 

JP and I discussed this a couple years ago because I couldn't get MC to backplot or verify a toolpath correctly although it would post correctly. My theory is "If it ain't broke don't fix it".

[Guest CNC Apps Guy 1]

The biggest benefit of using control (which I prefer as an operator) is the ability to see print numbers in the program...

Old school guys HATE my programs... no matching numbers ANYWHERE.

 

That is by design though. I don;t want operators rifling through my stuff. If there's a problem, let ME or another programmer handle it. That way it gets fixed not band-aided. If the MC file is right then things just go better in the long run.

 

Which reminds me if a time when I worked for a company where we had a shop supervisor that refused to deal with a particular night shift operator. This dude would tinker with every single program so us programmers go together and came up with a way to deal with him. LOL... we started setting zero always in the center of the stock, the we'd rotate the part slightly so what normally woudl have been a straight X move was now an XY move. Oh man... drove his nuts, he couldn't figure out anything anymore. Mysteriously things started running better once he kept his mitts off the programs.

 

JM2C and I'm sticking to it.

[Joe788]

We use wear on Mazaks. You can still use wear, and have the tool diameter showing in the Tool Data page. You just put the wear in the Tool Offset page. Depending on how the machine is set up, you might need to change some parameters to make it work the way you want, because there are a lot of different available combinations for telling the control where to look.