Contour with wear

[Harry Morse]

Using mill 9.1 I made a contour around a 2D part using wear setting left.

 

It appears to give me the opposite if I put a + value in the fanuc control to make the part smaller.

 

I checked in the help file which is the same as I got so I know I did it correct.

 

Looking at the help file explaining about wear and reverse wear the help file seems to be the opposite or reversed to what it should be.

 

Anyone else experience this or think this is actually reversed or am I wrong.

 

Thanks

[Fig sign]

Harry !

Welcome to the Forum !

Wear is a Cimatron type compensation ,when the toolpath is offseted like in type compensation -computer plus offest is implied

For tool end mill 10 offset 0(zero )and for every other tool too!!!

To take 0.1 offset -0.1 ,to take 0.1 less offset 0.1

It has some good points but I don`t like it and it can turn to the long argument is it worth to use it .

Just 2 words: _avoid using different types of compensation (control and wear ) for one tool ,avoid using different types for one program ,even better -always use one compensation type otherwise you are risking human fault and as

a result ->parts scrapping

quote:

---

¨ Wear – combines compensation in computer and control. Mastercam calculates the compensated positions based on the tool diameter stored in the tool library, and codes them into the position and feed moves in the NC program. It also inserts the G40/G41/G42 codes to turn cutter compensation on and off. In effect, the tool moves are compensated twice.

 

Wear allows for a wear offset (the difference between the original tool size and the reground tool size) to be applied at the control. The wear offset is a negative number entered into the tool diameter register.,,,

To use the Control, Wear, or Reverse wear options correctly, you need to make sure that your toolpath includes a move at the beginning and end of the toolpath to turn compensation on and off correctly. You can either extend the toolpath geometry to accommodate this, or specify lead in/out moves as part of the toolpath parameters.

---

HTH

If you still have more specific questions -

you are welcome !

eDIT : yOU r ALWAYS WELCOME !

 

[ 01-20-2004, 06:34 AM: Message edited by: Iskander teh Owl ]

[Harry Morse]

Thank you for the reply Iskander

 

But I should have been more clear in the help file it says

-------------------------

 

This is what the help file says:

 

Wear - calculates the compensation (1/2 the tool diameter) into the toolpath and also outputs a G41 code when the direction parameter is set to left, or G42 when direction is set to right. Wear allows for a wear offset, for example .001 (the difference between the original tool size and the reground tool size) to be applied at the control instead of a diameter offset. When the Wear option is selected, compensation in computer and control are both enabled in the same direction.

 

¨ Reverse wear - operates on the same principle as Wear, but instead generates a G42 when the compensation direction is set to Left, and a G41 when the compensation direction is set to Right. When the Reverse Wear option is selected, compensation in computer and control are both enabled, but in the opposite direction.

--------------------------------

 

So I used it as it says in the help file and it seems to do the opposite to what it says.

 

I agree that it is not a good way for offset but if you have a bad machine and you want the software to do the offset and just use the control offsets at zero and use a value to compensate for tool wear to save making a new program.

 

I agree it is not good and it is dangerous so we would not use it on other machines just one bad one.

 

So my query is the help file ok or is it reversed because it seems to be to me unless I am missing something.

[Nominal]

quote:

---

It appears to give me the opposite if I put a + value in the fanuc control to make the part smaller.

---

Are you saying that you put a positive value in the tool table on the control and you expect it to remove more material?

[SLJ]

We always use Wear, but define the offset(for the operator) as the difference between the actual tool size and the nominal value. example .740 dia. e/m, put -.005(radial set in parameters of control) in control dia. comp offset. You are basically telling the control that the tool is .01 smaller than programmed. The more "minus" the more you will take off the part. hope this isn't too confusing!

[Fig sign]

Harry .

Make rectangle 100*100 write contour toolpathes with dif. types of compensation ,post it and have a look .

U`ll catch it fast.

I can explain more verbose later !

HTH

[Thad]

quote:

---

The more "minus" the more you will take off the part. hope this isn't too confusing!

---

That sums it up.

 

The help file is confusing (if not wrong) when using a positive example for a resharpened endmill. If it's a resharp, it has to be negative.

 

If you use wear comp and you use the exact size endmill that you programmed for, then put in a zero diameter (or radius) in your offset page. If you have a resharp, put in (a negative) the difference bewteen what you programmed for and what you're really using.

 

Thad

 

[ 01-20-2004, 09:32 AM: Message edited by: Thad ]

[jenks]

This is rule of thumb that I use with a Haas control, which I believe works like the Fanuc:

 

First, zero out the tool diameter. Run the part, if any adjustments are necessary do the following:

 

HOLES:

 

To make the holes bigger use a negative value, such as -.001.

 

To make the holes smaller use a positive value, such as +.001.

 

OUTSIDE CONTOURS:

 

To take stock off the contour, use a negative value.

 

To make the contour bigger, use a positive value.

 

 

ISKANDER has a very good idea about the 100 x 100 contour. I used a variation on the idea to get comp operation perfected on every type of operation that I use. It worked with pockets, circles, OD contours, it took some effort, but the end product was worth it.

[TheePres]

As the name implies, cosider "wear" on the tool if you program to .500 diam and your tool has 'worn to .499 you have -.001 wear

[Harry Morse]

Thanks for the replies.

 

After seeing these replies it would seem that the help file and the settings are both actually wrong.

 

It would appear that the names Wear and Reverse Wear chould be reversed otherwise others like ourselves will make the part wrong unless they know that they are actually working in reverse.

 

I did the rectangle test as suggested and if you look at the code thats the way it reads anyhow.

[Andy]

Ditto Jenks

[Fig sign]

Why I don`t like wear and reverse wear :

They are dangerous IMHO

1. entering radius ofset senseless and not reflecting the tool size .

2.combining them with regular radius values can be confusing and can lead to crash

3.you are getting longer toolpath file size and filtering resaults will be worse than compensation -control

4 .the code not reflects the real part dimensions .it is hard to read (debug )

 

You can add more points but I think it explains why I don`t use it at all.

I can not find some good points to tell about it ,sorry

 

This is IMHO and I stick to it !

[P_Scott]

Iskander,

 

I mean no disrespect. I've always been taught that Wear is the best of both worlds when compensation is included in programming. Here are some reasons for using Wear instead of Control comp.

1. Easier and faster setup on first-run of any job. Operator input error is lessened if not eliminated. Tool size for ALL tools at setup is 0 (zero).

2. Easier adjustment of tool size at control IF tool wears down during machining. Rough tools need not be adjusted. Only finish tools need to be adjusted by the difference in what was programmed and what actual tool size is.

3. Easier replacement of tools. Tool breakage occurs. Put in tool of different size than called out for in program and make adjustment for difference in size at control.

4. Entry/Exit values can be less than 1/2 tool diameter. Tight spaces require the use of tighter entry/exit moves. Turniing comp on a line move that may only be 0.01 or 0.02 long is better than having to arrange a different approach with a line that needs to be equal or greater than tool radius.

5. Infinite look ahead and gouge checking features in Mastercam are more accurate with Wear comp than Control.

6. With Backplot and Verify tools in Mastercam, as well as 3rd-party products to verify code graphically, why read the code file for debugging? Use the computer to help check the code before sending it to the machine. I wouldn't want to read a code file line by line, no matter how short it is. I also don't see where you lengthen the code just by using Wear as opposed to Control comp. They're both adding the G41 or G42 to the code during posting. Where's it adding to the code using Wear as opposed to Control? JMHO

[Nominal]

I only use wear offsets. Other places I've been use in control. The problem with that is ( and it happened often enough ) was if someone forgot an offset they were half the cutter dia into the part. With wear if they forget an offset, the part stands a better chance of surviving. Yeah I agree with isky about being able to read the program easier, but then again maybe I don't want people reading the program just hitting the button. If somebody has got to read the code to that extent it usually means there are other problems anyway that they aren't going to solve nor do I want them to try without talking to me first.

[Eeyore-nonhuman forum member]

Peter !

I met Wol at noon and smoked with him a cigarette .

He said that he `ll be busy and asked me to answer instead of him today .

Although I am not so clever as teh Owl but some

answers can give even my humble person.

quote:

---

I also don't see where you lengthen the code just by using Wear as opposed to Control comp.

---

Gotcha!!!

Build simple rectangle 100*100 and make toolpath contour with CC control and with wear and after that backplot and save the backplot as geometry .

You will see that in control compensation You will have less enteties than in wear or computer type toolpathes .

Mastercam will build betwen every two nontangent entities arc and the number of entities will be greater .

And You don`t need to do even this just compare NCI sizes !

Filtering results will be close to zero with tooltype wear cause your have a consistent tangent toolpath .

About safety

quote:

---

Tool size for ALL tools at setup is 0 (zero).

---

You think it`s good ?!?

Just put instead of end mill 10 end mill 12 and mill a slot .Operator forgot to change offset ?Right !

quote:

---

. Operator input error is lessened if not eliminated.

---

That`s your words.

All is very relative .

About reading /debugging .

Good to read block or two before crash sometimes.

It saved me a lot of times .

No matter what was a mistake , you saved a part .

Well ,milling always one part I sometimes read it while running in critical moments .

It`s a waste of time to read next block on wear program !

It is not hard to remember to add radius in the setup ,in fact it disciplines an operator /machinist and you can always tell what instrument is working .

When you have dumb operators that can not divide diameter in two you can work wear !

If you want to add a couple of blocks by hand it is very disturbing too and even with a mastercam

and very good stable post I sometimes do it .

quote:

---

I don't want people reading the program just hitting the button.

---

And if you work both programming/machining ?

Or you made a mistake and now you check yourself ,"dear me" ?

I am with Iskander ,we both prefer to stay away from wear !

Yet I worked wear once too , .

 

Good luck ! I think I explained my point of view .

[Chris Rizzo]

Other than setting to wear, how else do you deal with re-sharpened tools, as opposed to re-posting the entire program with adjusted tool sizes?

 

Also, unless you are paying top dollar for full-size endmills, tools do indeed vary. Frequently tool manufactures will buy blank carbide stock at the dia. of the shank, and THEN grind the tool shape. A .250 tool coming from a .250 carbide blank cannot have a true .250 cutting dia. when finish ground....

 

But then again you put a .2498 tool in a holder with .0002 runout, and your once again effectivley cutting .250!

[JG]

This maybe worth noting, When having MC compensate for the endmill size AND you are doing an Internal contour AND you have a Fillet the same size as your tool in MC, your code will NOT have a arc in that corner.... so if you use a regring/smaller EMill your fillet will also be small.

 

I still prefer using wear, and start at zero for a offset.

 

Quick, check you jobs for internal corners !

[Eeyore-nonhuman forum member]

quote:

---

Other than setting to wear, how else do you deal with re-sharpened tools, as opposed to re-posting the entire program with adjusted tool sizes?

---

Come on ,you are killing me .

Toolpath for CC control for end mill 10 real 9.8

offset 4.9

Toolpath for CC wear end mill 10 real 9.8 offset -0.1

Toolpath for CC reverse wear end mill 10 real 9.8 offset 0.1

All of them will give you the same good result .

The question is whichj of them do you prefer ?

You know my preference .

[P_Scott]

Eeyore,

 

Wear or Computer seems to add entities in corners. That's due to "Roll cutter around corners" and only if you have "roll cutter" set to either "sharp" or "all". It's not the compensation switch that does that. Besides, if you're just sending a file to the machine to be saved in its memory, you're limited by the control's memory. If it's too big, you drip feed it. If you have twice the amount of entities for contours due to "rolling" of the cutter around corners it doesn't matter because it will still cut the same profile whether it's from the control's memory or is drip fed.

 

Rolling the tool will also maintain the chip load of the cutter and "de-burr" the part at the same time. That function is not available with control comp if there's no arc in the part profile. Then you've got to waste time de-burring the part after it's taken out of the machine. I'd rather have the machine do most of the work for me. Who cares if there are more entities. It costs less to have the machine do it than to have a person do it. If a person does it, you also won't get the consistency and repeatability of the machined result, no matter how good the person is.

 

With modern machine and sophisticated software tools, there's little reason to debug a program line by line. You should see a crash in the simulation of the program even before it's posted. While the Verify is running, you can check e-mail or do something else if you think it's taking too long. I'd much rather run Verify one too many times than crash the part in the machine because I was tired from reading repetitive lines of code and missed the line that caused the crash.

 

+1 JG. Add that reason to the list.

 

I'm sorry about the book. Just when someone says "gotcha" to something I was just voicing my opinion about, it tends to put me on the defensive. You do what you want Eeyore and Iskander. My point wasn't to attack your opinions, merely to show others some reasons for using Wear instead of Control. That's the beauty of Mastercam. It allows you to do what you want no matter what it is. You said it yourself.

quote:

---

All of them will give you the same good result .

The question is whichj of them do you prefer ?

You know my preference

---

 

[ 01-22-2004, 04:51 PM: Message edited by: Peter Scott ]

[heeler]

I really like to use full. Now that mastercam has the ability to do a plunge after the first move on the leadin/leadout I see no need for wear. I also ALWAYS put in the dia. of the cutter when putting the tool in the machine. It is just a habit that I do. I use the same process every time that I put tools in the machine, setup a part or setup a part in mastercam. One note to everyone using Fanuc controls. Parameter #5004 bit 2 ODI (The cutter compenstion value is a radius value = 0/ Diameter value = 1. We have ours set to a 1 so that we can just enter the dia. You can also set is to a .9999 value that would be a .49995 radius.

 

JM2C

 

Glenn

[Müřlıń®]

quote:

---

Other than setting to wear, how else do you deal with re-sharpened tools

---

Do like Rekd once said:

 

"Smack it with a hammer and make it run out more"

 

I think wear has to do more with high-production turning than milling.

 

Most of my programs are way too long to even worry about wear.

This is why I always buy the best tin coated micro-grain carbide available and use machining stratagies that do not require one to run a program, measure, add wear, re-run the prog.

 

I already know that my endmill(under normal conditions) is going to do what I tell it to do.

For High-precision parts you will want to use a new endmill anyways...Endmill breakage will most of the time, gouge an expensive part and the 20 bucks it cost me to put a new one in is worth every penny.

 

 

JM2C....

 

 

Murlin

[Fig sign]

Peter !

I want not to argue ,only to point something that may be interesting.

quote:

---

That's due to "Roll cutter around corners" and only if you have "roll cutter" set to either "sharp" or "all". It's not the compensation switch that does that.

---

NOr that it really matters ,it`s not so true ,IMHO .

Roll cutter around corners is what CC control compensation does on machine ,IOW machine tool controller does .

It simply builds radius offset vectors and builds arcs over corners .

This is default type of compenstation on most machines .

No need to argue ,just see a compensated toolpath trace over alluminium plate once and you know what I mean .

All types of compensation ,limitations of geometry calculation and buffer limitations were discribed very nice in superhit of all times 'Yellow book of Fanuc6"

Sinse that time nothing changed in principle.

So may be everyone has rs232(V24) 55600 like in my new machine, or even better ethernet cards ,wireless, but at my antic one I have 4600 and very limited memory and I run it.

So may be a growth of file size has a sense sometimes ,but aniway it is interesting and funny ,isn`t it ?

I write about it from pure fun ,but may be once someone `ll make use of it anyway and would say me thanks .

To say

quote:

---

Who cares if there are more entities.

---

If you mill a very accurate spline built from a huge ammount of points and you can not filter it due to CC wear it also doesn`t matters noone ?!?

Everyone has data servers and huge buffers so it not matters that feed can fall 10-30 times and more because of buffer not big enough for movements execution ?!?

Why I know about this things ?

I read programs .If I run a program and my toolpath consists of only lines ,you have CC wear and every second block is arc you became at first at least curios and then find an explanation !

May be also because my machine tool if I open the door -spindel falls 0.03 mm and to work without door interlock is a suicide I can not look on what happens on now and I read program on line on critical situations .

Wear is the only type of compensation available in Cimatron and they are arguing with me 7 years if no more and were not abled to succeed.

I had not heard today nothing new in principle.

I can explain every point by point every staitment but it gonna turn to spam.

So I return to the Wolery.

[Harry Morse]

Thanks for your replies

It appears that it is best not to use this wear function at all.

 

On further investigation I have not been able to find this method in any of our machine tool handbooks.

 

this being the case why is the function there or how did it come about.

 

Does anyone know of a machine control that recomends using it this way.

 

It would appear from what I have learnt here it is a recipe for disaster to use it.

[Fig sign]

Machine buiders can say anithing they like that `s you to select .

Yet I know of at least one Cad-Cam package thaT HAS only wear :

Cimatron - Both Cimatron IT and Elite .

Cimatron .

And I know ppl working full times Cimatron programmers really happy with it .

You can get used to anything the question is what will u get and loose ?

And the understanding of the fact that jumping from CC type to Type can cause scrapping .

Set in operations defaults CC type you prefer for every toolpath together with other settings and you` ll be happy.

 

I like the old saying from Talmud that it is not permitted to believe in anithing that human mind can not explain

[MACHINEMASTERG]

harry i dis agree ...wear is the standard here program in mcam for the tools dia and let mcam do the comp and use wear with a 0 set in the controllers offset page and then you can dial the parts dim in with like .001 or -.001 etc... etc in our place wear is where its at