Cutter Compensation in surface toolpaths

[Chappyd]

Hi, I have a kinda noob question about cutter comp. I made a program using surfaces for the 1st time, and it looks pretty good. Except when I post it out, I do not know how to compensate for odd tool sizes. There's no G41, and that's about the limit of my experience with cutter comp.

 

When I make a 2-d mill program, I have always selected "wear" in the cutter comp type window. Here in our shop we do that and allow the operator to adjust the part size using positive or negative values, and the program always posts a G41 and Dxx.

 

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?

 

Thanks

 

Chappyd

[800mxz]

That is becasue most controls can not do 3D cutter comp.

 

If tool size changes the surface will probably have to be re-posted.

 

IMO - best to use on size tooling for surfaces

[Guest]

resharp tool and 3D surfacing????

 

 

You would need to program it based on the size of the too going to be used.

[Ocean Lacky™]

As far as I'm aware, this is not possible on a surface toolpath. You would have to enter the new values for the reground tool in your tool parameters page and then regenerate the program.

[Chappyd]

Well, I guess that explains that, lol.

 

Thanks very much for the quick replies.

 

Chappyd

[Guest CNC Apps Guy 1]

Everything is possible...

 

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.

 

JM2C

[800mxz]

Proceed with caution on adding g41 manually, surface geometry accuracy will vary (the more comped away from true diam. the more inaccurate the surface)

[Darren Long SPE]

I think on Heidenhain you can have 3D tool offset.....im trying to remember is it M118 or G118 ......been a while since i needed it.....

[Thad]

quote:

---

WHen I need Comp on a surface, I go into "Direction" (on old style toolpaths)...

---

If James says it's so, then I'll assume it's so. But I won't assume that the direction option works! It doesn't on pencil toolpaths. I reported that one to QC a while back.

 

Thad

[MultiAxGod]

quote:

---

Everything is possible...

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.

---

That does not work!

 

 

quote:

---

this is not possible on a surface toolpath. You would have to enter the new values for the reground tool in your tool parameters page and then regenerate the program.

---

quote:

---

Proceed with caution on adding g41 manually, surface geometry accuracy will vary (the more comped away from true diam. the more inaccurate the surface)

---

Both are true. The cutter is very rarely at the edge. Comp only works on the side NOT the tip or any part of the ball, so your surface will be inaccurate. If you are making a mold or airfoil and must maintain surface accuracy, then you will have to program it for the ball radius that you are using.

[Thad]

quote:

---

Comp only works on the side NOT the tip or any part of the ball

, so your surface will be inaccurate.

---

Years ago, I programmed surface-type toopaths by hand. They typically cut angles and arcs in the G18 or G19 plane, then did a straight step over and cut back in a surface-finish-parallel fashion. 2.5D, I suppose. I programmed them on a Fadal with a ball nose using G41 and G42. I set my tool length to the center of the ball and the Fadal comped it. Now, that's isn't exactly MC programming a surface toolpath with comp, but the toolpath cut dimensionally correct. So I disagree with the part of your quote above that I made bold.

 

Thad

[MultiAxGod]

quote:

---

So I disagree with the part of your quote above that I made bold.

---

While I can agree that if you program your path to the center of the tool AND your ball is the correct diameter, in theory, it SHOULD be correct. Sorry, I just won't/don't have time to explain a very different style of programming and machining and explain that an operator has to make sure what is correct and what can vary. If I was doing it myself, I could do all the fiddling to make sure it was accurate, but I wouldn't add this to a "machinist's" ,giggle!, plate! Especially if the name of the game was production. Unfortunately, this is the viewpoint I commonly take when analyzing what will work and what won't. My view has always been to make a program that anyone can walk in off the street and run and understand to the "standard" methods.

I have run across many surfaces where this method will not work, though, for the type of surface and the style/accuracy of the cut. As a matter of fact this was a big hold back to Mastercam sales a few years ago that the core math was a two dimensional system which is what the method you are describing above is, and could not do proper compensation on a ball or bull tool. The method above ONLY works on a ball and will not work on a bull nose tool.

I know this will open Pandora's Box, but que sera, sera!

 

My own opinion is that ALL setups/programming, software set ups etc. need to adhere to the commonly used industry standards so that a company can survive lay offs, walk outs, God forbid Death, etc. and still keep producing.

[Thad]

quote:

---

While I can agree that if you program your path to the center of the tool AND your ball is the correct diameter, in theory, it SHOULD be correct.

---

Maybe this is what you meant, but I programmed to the print dimension and let the machine comp for me. Kinda like using control comp on a 2D MC program.

 

 

I was simply challenging your statement that it won't be accurate using cutter comp on a ball where the cutting action is anywhere on the ball other than the edge. I'm not referring to a production type setting, how much money can be made on the job or if I'd even recommend cutting anything that way. I'm just saying that it will cut dimensionally correct with an onsize OR resharpened ball.

 

You are also incorrect about using a bullnose. There are limitations to *what* can be cut, for example, you could not cut a V shaped wedge with a rad in the crotch. Set your tool length to the center of the corner rad and then use a fixture off to offset the distance from the center of the tool to the center of the corner radius. It is then programmed as if you're using a ball with the tools corner radius. So if you were using a 2" dia with .250 corner rads, your diameter offset would be .250 and your fixture offset would be .750. I've done it and it comps accurately.

 

Thad

[Thad]

BTW, with a bullnose, it gets more interesting if you have to change which edge of the insert you're cutting with. Imagine cutting a letter A that is standing up. Starting on the right side and going up the angle, you're programming for the front edge of the tool. As you hit the peak, you have to pick up another fixture offset so that you're programming the back edge as it cuts down the other side of the A.

 

Thad

[800mxz]

G41, G42, and G40 are all for G17 compensation (Compensate in the X&Y) with no Z comp.

 

Yes the Heidenhein, Siemens 840D, and a couple other controls are capable of 3D comp, but they don't use G41 or G42 to execute it.

 

I have run a Hermle 5 axis that we had here on our floor, and programmed it with a .5 ball, and setup a simple X&Y toolpath that faced a 4"x8" peiece of material with that tool, flat with a .005 step over.

 

Start the program with the A&B axis flat, and let the machine move X&Y, and WHILE RUNNING THE PROGRAM, you could put the machine in hand jog and move the a axis and the machine would compensate the centerline of the tool center ON THE FLY. Then you select the B axis and start rotating the part on the other axis, and the machine could compensate all 5 axis at a time.

 

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

 

Most machines can only comp in the X&Y axis. Even if you turn on G41, then start moving the Z, the Z will move, but it will not compensate for it.

[MIL-TFP-41]

quote:

---

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

---

Siemens has been doing this for a while now with the TRAORI function & Fanuc has developed their TCPC function as well, but AFAIK, it is only available on the new 30i & 31i controls. Way cool stuff but it warps your mind trying to understand how it works.

[Guest CNC Apps Guy 1]

quote:

---

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

Everything is possible...

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.

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

 

That does not work!

---

 

If I had Camtasia I'd prove it. I know it works because I've done it. I didn;t hear about it, read about it or anything else about it, I DID IT, I figured it out myself and did it. So there

[acam]

3D compensation is supported on Mazak Matrix control. The NC program must include XYZ coordinates of the toolpath points and UVW coordinates of the points that represents the vectors that is normal to the part surface.

 

Mastercam is able to support this kind of compensation through comp3d.dll chook.

 

Of course this must also be supported by the postprocessor.

[Thad]

As the old saying goes, people who say it can't be done shouldn't get in the way of those who are doing it.

 

Thad

[MotorCityMinion]

You tell em' Apps guy!

[MultiAxGod]

Sorry to all of you, but your part might "look" like the picture, but mathematically it's not correct and no software is going to show you that, true surface mapping mathematics will. 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!

Close, but not "correct"! By the way there is a big difference between true 3-D compensation and 2-D comparison math.

I'd like to be proven wrong and belive that it's that easy, but many have tried for years while I was in the field around the world but all failed.

Don't mean to pi$$ any of ya off but that's the facts ma'am!

[MMT-USA]

Control Specific,

 

3D compensation will work for tool-paths all at one directional vector.

 

Re-posting the tool-path is necessary for a true 5-axis surface tool-path which the directional vector is constantly changing.

 

Left/Right tool offset is available for 5-axis swarf cut compensation but this is strictly cutter diameter.

 

There are new options for some controls coming out that need specific CAM support as you have to output two vectors, tool vector as usual and a vector from the tool center to actual tool cutting point so that the control knows in which direction to make the offset.

 

I believe I know one CAM system currently that can support this.

[Guest CNC Apps Guy 1]

I re-read the original post to make sure I understood what he was looking for.

 

I interpreted the question as CAN you have comp output on a surface toolpath. The answer is an emphatic YES. By the method I stated above.

 

When/if you comp, will the results be what you expect? That's a whole other question and can only be answered on a feature set by feature set basis. Like I said before, I have successfully done this and achieved accurate results at least according to a Zeiss CMM it measured within .0006" on profile tolerance - granted it's not .0001 but that's a pretty tight tolerance on a surface profile callout. I did it on on certain types geometric features with Surface Finish Flowline toolpath using the method I described above. With all that being said, will it work accurately and as expected on every feature you try? The answer is going to be a no for many of the reasons mentioned above by other forum members. There is no "one size fits all" solution to much in this world and if you want to accurately comp reground tools you're going to need to pony up some big caysh for a couple things, 3D Comp on your machine control, and a pretty tricked out post Processor to control all that.

 

quote:

---

...There are new options for some controls coming out that need specific CAM support as you have to output two vectors, tool vector as usual and a vector from the tool center to actual tool cutting point so that the control knows in which direction to make the offset.

 

I believe I know one CAM system currently that can support this...

---

Powermill?

[MMT-USA]

What forum are we in?

[Guest CNC Apps Guy 1]

We don;t have to deny the existance of other products. If another CAM system has a feature that is vavaluable it's not a sin to mention it. I know I've done and said FAR worse (at least regarding the Lathe Product and it's NUMEROUS deficiencies) DOH, I did it again.