Cutter Compensation in surface toolpaths

[mowens]

I've worked at one shop that used 3D compensation; unfortunately I don't remember what control they used. (It was 4 years ago and I'm old.) Most of the machines were Cincinnati single spindle 5 axis. The software was Catia V4; I do remember about the 2 vectors.

[chip]

C:/mcamX/documentation/whatnew.htm#_CAD_file_for_Compensation_for_Surfaces

 

Should be on most of your desktops when one installs McamX.

 

I'm having trouble uploading files to my photobucket.

[chip]

 

[MultiAxGod]

Maybe I missed the point in the original post but it seems to me the question was why doesn't he get G41, G42 when he outputs a 3-D Surface? Because it will NOT work on 3-D surfaces. You have to comp (albeit, bad choice of words) for the individual tool in the CAM Software. This is a multitude of data being calculated dependent upon where exactly the cutter is contacting the surface. It is generally constantly changing.

Could I write a toolpath guaranteeing that 2-D comp values would work,,,,SURE,,,,BUT WHY would I?

Nobody disputed that it's not in the software Chip! This is the correct way to get good numbers. If you change the tool rad, dia. etc., you must redo (pick a new tool description that describes the new tool) and re-post.

Sorry James, but I still disagree, unless you are cutting always in one direction and maintain the exact same point of contact with the cutter, which on a 3-D surface is a rarity. Yes, You or I, can make a million work arounds to do things certain ways, just because of our experience, and spend hours upon hours redoing things, which if you do the following method, only takes a few seconds. But the general rule, especially for people that do not understand 3-D mathematics, is an emphatic "NO". Unless I am completely missing Chappyd's question.

Simple....Done....finito....End of story!!!

 

BTW, in a control, this type of compensation (3D tool vectoring and 5 axis comp) is a patented process One company owns it and it's NOT Fanuc or Siemens or Vickers or Mazak or Mach or xxxxor, etc.

[chip]

quote:

---

Just a simple man with a simple plan!

---

[chip]

quote:

---

.... why doesn't he get G41, G42 when he outputs a 3-D Surface? Because it will NOT work on 3-D surfaces.

---

Here is my theory..... It is only a theory. The software is needed to generate the code for the surface(s) to be comped. If One has the proper code that is generated. i.e. creating arcs and room to turn cutter comp on and off...

 

 

quote:

---

WHen I need Comp on a surface, I go into "Direction" (on old style toolpaths), add a linewith an angle on entry and Exit. Then go into the toolpath editor and edit the point where the lead in line and turn cutter comp on, then go to the end and turn it off.

---

....instead of having to imput this code manually. The control (I am learning the only control on earth)....

 

quote:

---

To this day this is the only machine/control that could do a "true" 5 axis comp.

---

Should comp the program. Weather the cut is in a G17 (XY), G18(ZX), G19(YZ) and the only control on God's earth that could calculate such incrediable numbers should take that arc or code and comp the numbers. It is not a secret that the compensation is at the control.

 

This control shouldn't care what plane it's in. It should take that number from the program and shave a couple thou or add a couple thou.

 

quote:

---

Laws of physics apply to machining and math doesn't change. Close just isn't close enough in the fields I've worked in, especially for surface mathematics and this "it worked" theory has been proven wrong mathematically ever since data points were first put together and surfaces were cut point to point with a ball or bull or straight or any other type of cutter. Sorry guys!

---

Seems to me that you must know a lot!

 

The boys that have interfaced MasterCam have done a good job with their product!

 

I am sort of old school and should I need to make some adjustments i.e. electrode or surface adjustments I tend to use stock to leave or change the dia. of the cutter.

 

I'm still learning to read.....

 

quote:

---

Using the surface toolpath options, my only comp options are tip, & center. Could anyone enlighten me or point me to a source where I could educate myself on how to use this so the operator will be able to change values for resharpened tools?

---

My anwser would be that from what I have learned... Version X has the capabilities to comp surfaces. I could still be incorrect in this.

 

Should your machinist re-sharpen his e.m. and you need to comp for the adjustment. I would recommend you change the .NC code if you are un-familiar with this new function!

 

Didn't mean to step on God's toes....

[Mic]

12 years ago!! I used true 3D cutter compensation on a Matsuura MC-760VX with a fully loaded Fanuc 15M controller. I can't remember if we used G41 or G41.something. But all G1 lines had XYZ + IJK witch was the vector to do the compensation along. We used a cam system called ICEM DDN and programmed a 5X toolpath normal to the surface, that way we got the correct vector. And tip comp was of course set to center.

 

We used it mainly for machining edm electrodes. That way we could change the gap without changing the program.

[Guest CNC Apps Guy 1]

quote:

---

...Sorry James, but I still disagree...

---

After WESTEC I'll put up a sample MC file, and code output to prove once and for all you don't have to edit code to put cutter comp on a Surface Toolpath.

 

Do you like your crow with feathers or without.

[MultiAxGod]

quote:

---

This control shouldn't care what plane it's in. It should take that number from the program and shave a couple thou or add a couple thou.

---

You just stated the magic words, it shouldn't matter what plane its in. G41 and G42 are planar only. G17 or G18 or G19. A surface is in 3-D going through the 2-D planes. G41 and G42 do not work. It's as simple as that. Think about cutting a surface, the point of contact on the surface is generally, constantly changing and while it may not be much of a movement it is still movement out of the (typical) G17 plane.

 

 

quote:

---

This control shouldn't care what plane it's in. It should take that number from the program and shave a couple thou or add a couple thou.

---

It only shaves or ad's in the plane that it is set in, not all 3 axis (or more depending on what you are machining with). The only control that does this, has a patent on the concept and must have the 3 D vectors included with the G-Code to apply it. What happens when you have .01" comp set and the machine only moves .001" I wonder? And how does it work when the cutter comes back the other way, now the comp is in the opposite direction and you are gouging your surface. HOW DOES IT KNOW WHICH WAY TO GO?

 

 

quote:

---

Seems to me that you must know a lot!

---

Not in most areas! LOL! But this one I do!

 

 

quote:

---

My anwser would be that from what I have learned... Version X has the capabilities to comp surfaces. I could still be incorrect in this.

---

This is the correct method. The control does not comp 3-D surfaces.

 

 

quote:

---

Didn't mean to step on God's toes....

---

Don't worry, I keep 'em well hidden just in case! Got to....from Apps Guy! ROFL!

 

 

I give, you guys cut it your way and I'll cut it mine! Works for me! LOL!

[Guest CNC Apps Guy 1]

Here it is... I got a few minutes.

 

Linky

Mastercam Part file, and Code. I used the generic FANUC post. nothing fancy.

 

Username: mastercam

Password: swiss

 

[MultiAxGod]

quote:

---

Here it is... I got a few minutes.

---

LOL! I guess I don't know what to tell ya my friend. It will be close, but it won't be accurate!

Change that radius a micron and oops! It just keeps getting worse the farther you go with cutter changes. It doesn't matter the surface unless its just a straight plane and you are doing a planar cut that is always on the same side at the same point of contact going the same direction, well, that would be a 2d cut, I suppose. That's just the math of it. 2D cutter comp doesn't work for a 3-d surface.

If your point was to "force" a G42 into the program .....I give, I give!!! ROFL!!!!

Hey, just out of curiosity, what happens when it drops down and comes back the other direction?

 

Not right, So Solly!

 

Again, you do it your way and I'll do it mine!

 

[Guest CNC Apps Guy 1]

My entire point was that you could get G41/G42 output on a surface toolpath. As for if it will be right or not, you have to take it on a case by case basis. Since I have all the tools necessary at my disposal to do full 3D comp.I would only do the method I showed if in a pinch and if there was sufficient tolerance to do so.

[MultiAxGod]

MERCY!!!!! UNCLE, UNCLE!! LOL!!

[Storkman]

3d comp

 

Here is a link to a patent. Issued in 1996. Assignee: Fanuc Limited.

[800mxz]

MultiAx- Thanks for backing me up.

 

G41 and G42 only comps in X&Y, no Z compensation. Change Diam. by .02" and your part will get wider or narrower, but will not get any taller or shorter.

[MultiAxGod]

Just because you CAN force a code on to it, doesn't mean that it works nor is a good idea!

[Guest CNC Apps Guy 1]

Never said it was a good idea but worked perfect on the particular application I needed it for.

[Thad]

quote:

---

G41 and G42 only comps in X&Y, no Z compensation.

---

That is only correct in the G17 plane.

 

Thad

[mowens]

The G code for 3d cutter comp on the machines I used it on was G41.2 or G41.6 (G42.2 or G42.6). This was on a Fanuc control. It requires a vector to be output on each point.

[Guest CNC Apps Guy 1]

Thad stirrin' the pot

[Bruce Caulley]

I'm with Multiaxgod on this one. James' workaround will "work" if you are "compensating" for a couple of microns difference in tool diameter. I.e programmed for 12mm ball, actual is 11.987. The error induced in this case would most likely not put many parts out of surface tolerance. BUT, programme with a 12mm ball and decide to run with a 10mm and the surface will vary from 0 to 1mm out of spec depending on where it is measured.

 

So no, g41 g42 won't work on 3d. MC doesn't have a 3d comp button, and comp to surface isn't the same thing.

 

Bruce

[Guest CNC Apps Guy 1]

The exact situation I tend to use this workaround is when I'm using full radius keyway cutters that are HSS. They are RARELY the size as advertised anyway, I program it for nominal size, the radius is full so that's ok. Anyway, I need the comp so I can get the feature to correct size. As I always say, you have to take things on a case by case basis.

[Post dept]

All,

 

We have run 3D comp (for ballnose cutters) on surfacing tool paths on several controllers from our posts. At this time we can only get the data from Mastercam on 5-axis surface paths.

 

This is not to be confused with G41.2/G42.2 which is control/wear comp for swarf cutting (endmills). This can be run on any path because you can add a misc integer to force comp output even if Mastercam doesn't have a dialogue box for comp selection.

 

Brett