CUTTER COMP PROBLEM

[DCOPE17]

I have no problems doing what you're wanting to do. Why do any arc moves if you don't need to. 

 

I however, un-check Entry and Exit

 

I then check Adjust Start and Adjust End of Contour and add my desired lead in amount there. I have always gotten 3 lines of code.

G41 G1, then my G40. 

 

I never add to any geometry ( If I don't have to ) that doesn't work well if you get a new revision of the model and have to go re-create those modifications. 

[Thad]

What sort of problems can I expect? Educate me.

 

Gouges, code that won't run, unexpected moves at the machine that you don't see in backplot, possible crashes with nearby part features, etc. The mere fact that we're here talking about it should tell you something.

[Leigh @ Kodiak]

Gouges, code that won't run, unexpected moves at the machine that you don't see in backplot, possible crashes with nearby part features, etc. The mere fact that we're here talking about it should tell you something.

I can see how these would be of concern if my D comp in the control was set to the radius of my tool, but if I'm only using wear compensation, none of these things are ever going to happen.

[Thad]

I can see how these would be of concern if my D comp in the control was set to the radius of my tool, but if I'm only using wear compensation, none of these things are ever going to happen.

 

Then, by all means, carry on!

[Leigh @ Kodiak]

Then, by all means, carry on!

 

 

I think I will. My 17 years of programming without this ever causing incident is more than enough to make me confident that I'm doing nothing wrong.

[Thad]

LOL

[jlw™]

 

 

 

 

I believe some one's feeling is hurt.

[Leigh @ Kodiak]

LOL

 

Right back at ya. 

 

You can claim gouges, crashes etc all you like, but without an explanation of WHY they would happen, your are just throwing things out there.

[Leigh @ Kodiak]

Please explain why the path on the left would gouge, crash or otherwise be a problem compared to the path on the right, using wear comp. 

[Guest]

Put a value in the comp register......in the machine...then watch the numbers on the screen

 

increase and decrease it and watch how your comp engages.....depending on the value, your comp will start by cutting a taper as it engages..

 

This is why it is better and really just about an industry standard to engage your comp on a lead in move ...

 

My boss does the same thing here and it drives my nuts because the guys downstairs will use different cutters based on what they have....in tight areas, because of the way he uses it, it's not uncommon to have scallops on walls......change to a proper lead in lead out...the issue goes away.

[Leigh @ Kodiak]

Put a value in the comp register......in the machine...then watch the numbers on the screen

 

increase and decrease it and watch how your comp engages.....depending on the value, your comp will start by cutting a taper as it engages..

 

This is why it is better and really just about an industry standard to engage your comp on a lead in move ...

 

My boss does the same thing here and it drives my nuts because the guys downstairs will use different cutters based on what they have....in tight areas, because of the way he uses it, it's not uncommon to have scallops on walls......change to a proper lead in lead out...the issue goes away.

 

Yes, I understand how cutter comp works. There already is a lead in and lead out in that picture, they are co linear with the cutting portion. 

 

G41 D8 X-1.5365 F80. (LEAD IN MOVE, TURN ON CUTTER COMP)

X-.2083 (CUTTING MOVE,)

G40 X.0354 (LEAD OUT MOVE, TURN OFF CUTTER COMP)

 

Is there something I am missing? How is the "cutting move" going to get a gouge? 

[Guest]

RIF is fundamental

 

As long as your comp in the machine is 0 you won't see it...

 

As I said, put a value in the control and watch your numbers at the control......with a large enough value you will see it cuts a taper in XY

 

Don't look at the code, look at what happens AT THE MACHINE when you put values in

[Leigh @ Kodiak]

Of course it will make a taper durring the lead in move, but this is OFF THE PART, so it is not a problem. Are you saying it will cut a taper on the second position as well?

[Guest]

Of course it will make a taper durring the lead in move, but this is OFF THE PART, so it is not a problem. Are you saying it will cut a taper on the second position as well?

 

If the line is not broken and the comp move is large enough "it can" continue the comp move onto your part..

or you can get a scallop when trying to use a bigger endmill..those cases are more rare

 

If you do what you do under the right circumstances, it works, as you've seen.....it's just that in other circumstances "it can" bite you...

 

Using a perpendicular lead in move negates that possibility....

[DCOPE17]

RIF is fundamental

 

As long as your comp in the machine is 0 you won't see it...

 

As I said, put a value in the control and watch your numbers at the control......with a large enough value you will see it cuts a taper in XY

 

Don't look at the code, look at what happens AT THE MACHINE when you put values in

 

This always happens anytime you use CC and have a value other than "0" in the tool parameter. even with a Perpendicular entry, you need to have a "line" before the "arc" ( except a few machines, They can actually turn Comp on with an arc move )  and in that line you'l get the same taper movement but like mentioned above, its not in the part yet. 

[absolute technologies]

FYI

 

There is a Fanuc #5000 parameter that dictates whether the control compensates by moving the tool or shifting the coordinate system. This setting is the reason that you see machine having a tapered move when only 1 axis  is programmed, regardless if you programmed compensation perpendicular or not. We have several vintages of Mori Seiki machines here and they were setup different by Mori but I've since corrected them so they don't taper.

 

personally I'd have chit fit if my code had 3 X-axis moves in a row, I would have to totally re-do it.. no doubt!

 

Cheer!

Len Dye

[civiceg]

The company I used to work for, the standard was a 10 degree tangent lead in/out, whenever possible, with wear. When using small diameter tools, say under 1/16 and a small percentage for arc/length, MasterCam will not correctly apply comp because the change in one axis is so close to zero. Having said that it is not a software issue, but an input issue. I have seen this bite people, most of the time it just needed to be reposted with a more drastic angle. 

[gms1]

Put a value in the comp register......in the machine...then watch the numbers on the screen

 

increase and decrease it and watch how your comp engages.....depending on the value, your comp will start by cutting a taper as it engages..

 

This is why it is better and really just about an industry standard to engage your comp on a lead in move ...

 

My boss does the same thing here and it drives my nuts because the guys downstairs will use different cutters based on what they have....in tight areas, because of the way he uses it, it's not uncommon to have scallops on walls......change to a proper lead in lead out...the issue goes away.

Never once in the 20 years I have been doing this have I seen a control ignore the comp line and continue to comp while making the actual cut without the code to support it. I use wear, and I often times use tools that are a lot bigger than what I programmed (ex: programmed for 1/2, end up using a 3/4 with comp). So long as that first line the entry comp line has enough room to move you cannot see a tapered comp cut across your part. The code just isn't there to do that. Now, if you were to go full retard and put a 1in tool in where I programmed a 1/2 tool then yes you are going to have some serious problems.

 

edit:: I do typically like to give a nice 30 degree with arc on/off on most cuts but there are plenty of toolpaths that are just straight on and off.

[Guest]

Never once in the 20 years I have been doing this have I seen a control ignore the comp line and continue to comp while making the actual cut without the code to support it. I use wear, and I often times use tools that are a lot bigger than what I programmed (ex: programmed for 1/2, end up using a 3/4 with comp). So long as that first line the entry comp line has enough room to move you cannot see a tapered comp cut across your part. The code just isn't there to do that. Now, if you were to go full retard and put a 1in tool in where I programmed a 1/2 tool then yes you are going to have some serious problems.

 

edit:: I do typically like to give a nice 30 degree with arc on/off on most cuts but there are plenty of toolpaths that are just straight on and off.

 

Were you trying to make my point?  

[gcode]

One thing to keep in mind.. many of the old timers here started using CDC when it was in it's infancy.

It was not nearly as robust and forgiving as it is today

You could do everything right and still get burned.

I've been doing this 40 years now. The first NC machine I ran did not even have CDC,

If you had an undersized endmill, you rewrote the program.

The CNC's I started on would burn you to the ground turning CDC on with a straight line parallel move.

It may work today, but I'll stick with the  old school rules where CDC is concerned.

That doesn't mean the guys that don't are wrong though.

[Charlie Pierson]

I have been around for a few decades now and it seems to me that the 2 cardinal rules in applying CC are:

1, Turn CC on in straight line moves (most controls would probably alarm out on a arc anyway)

 

2, Most importantly, the CC turn on block should be non-cutting. ( as well as the turn-off )

 

Wear comp , perpendicular lead-ins (non-cutting), and only using the arc entry when needed (middle of contour, etc)

have always worked for me.

[Newbeeee™]

I think a huge amount of this is also down to vintage of machine control and also how the MTB has configured the parameters.

I have learnt that in this game safety is king.

Just because a problem has never happened to you doesn't mean your working to a safe process.