Radius issues, file.

[kretallick144]

Complete file from fusion.

[akash.kamoolkar]

I'm not referring to simulation graphics, when I output NC code using the Fanuc turning post processor I get linear moves for the first fillet  and an arc move for the second fillet. That's an issue.

Akash

[Anonymous]

Below is finish pass generated in Fusion using Haas post.

Rule:

When tool cuts inner arc, tool path results in tool radius being subtracted from one on part.

When tool cuts outer arc, tool path results in tool radius being added to one on arc.

To get R value from known I and K, take a square root of I square + K square

If only I or K are given, either is equivalent of R value because the other is zero.

Code marked in red is Fusion produced section of tool path that cuts two fillets.

Code marked green is produced in Inplot editor, I added radius value in parentheses which is equivalent of I and K values for illustration purpose.

When green code is plotted, tool edge follows each arc precisely, when red code is plotted tool misinterprets both arcs as you can see in graphics.

Both arcs are 1 mm and you can see that numbers correspond to the rule if you add or subtract tool radius from part fillets.

If you compare graphics of tool path produced in Fusion and Mastercam in my previous post you'll see the same problem.

%
O1002 (NIPPER HEAD 0O3)
N10 G98 G18
N11 G20
N12 G50 S6000
N13 G28 U0.

(PROFILE4 2)
N14 T0404
N15 G54
N16 M8
N17 G98
N18 G97 S866 M3
N19 G0 X2.2047 Z3.9764
N20 G50 S2000
N21 G96 S500 M3
N22 G0 Z0.0557
N23 X0.4503
N24 G1 X0.2785 F0.003
N25 X0.1672 Z0.
N26 X0.168
N27 G18 G3 X0.3097 Z-0.0709 R0.0709
N28 G1 Z-0.4921
N29 X0.3406
N30 G3 X0.4823 Z-0.563 R0.0709

N31 G1 Z-1.5497
N32 X0.4828 Z-1.5518
N33 X0.4844 Z-1.5537
N34 X0.487 Z-1.5553
N35 X0.4903 Z-1.5566
N36 X0.4941 Z-1.5574
N37 G3 X0.6004 Z-1.626 R0.0709

G1 X.4822 F.003
Z-1.526
G2 X.5296 Z-1.5566 I.0316 K0. (R.0316)
G3 X.6004 Z-1.6023 I-.0118 K-.0457 (R.0472)

N38 G1 Z-2.6181
N39 X0.8031
N40 G3 X0.8577 Z-2.6339 R0.0315
N41 G1 X1.4646
N42 G3 X1.5091 Z-2.6431 R0.0315
N43 G1 X1.5564 Z-2.6667
N44 G3 X1.5748 Z-2.689 R0.0315
N45 G1 Z-3.3031
N46 X1.6862 Z-3.2475
N47 X1.7323
N48 G0 X2.2047
N49 Z3.9764
N50 G97 S866 M3

N51 M9
N52 G28 U0. W0.
N53 M30
%

[akash.kamoolkar]

@Anonymous the nose radius of the tool in your plots is nowhere close to the radius of the tool in the file attached to this thread. Yours is much smaller. Not sure where you got that radius from. This is the tool in the OP's file with tool nose radius 0.8 mm.

[Anonymous]

Duh,...... I mistakenly used .008  tool nose radius in inch and I just now realized it.

The whole parade is result of mistake in tool radius and unit, .0312 radius on tool does prove out except for the incremental line moves rather then one arc swing.

Sorry for the confusion, as for original poster, free software leads to manipulate code and back plot tool paths are still good.

[Anonymous]

I have to correct you on one thing, imaginary tool point is point of intersection between two lines intersecting each other at 90 degrees, as shown, not two lines relative to insert geometry.

[akash.kamoolkar]

@Anonymous What you are describing is the Fusion "tip tangent" compensation type. However, the OP has set his tool to "tip" compensation type which is the intersection of the insert sides.

Regards,

Akash Kamoolkar

[Anonymous]

---

@akash.kamoolkar wrote:

@Anonymous What you are describing is the Fusion "tip tangent" compensation type. However, the OP has set his tool to "tip" compensation type which is the intersection of the insert sides.

Regards,

Akash Kamoolkar

---

Sorry, I never heard of such thing in 30 years. In every software I used before Fusion, tip assumes sharp tool point with no radius which is used in combination with "in control" compensation.

With such programming software outputs direct code relative to print dimensions with G41/G42/G40 codes and user must enter correct tip number and radius into geometry offset page of machine control.

Turning tool is #3, boring bar is #2, back turn is#4 and back bore is #1 etc.... there are tips from 1 thru 8 and center is zero or 9.

"In computer"  compensation uses tip tangent or "imaginary tool tip" where all compensation for any arcs and angle cuts is calculated in fixed numbers and changing to different tool radius requires reprogramming tool path.

Here is where things get interesting, if your claim is correct than 35 degree, 55 degree and 80 degree tools would have drastically different point relative to their geometry angles.

Now when machinist touches tools to probe or using "cut and measure" method, each tool would have error based on position of intersecting lines being programmed but not in sink with the way tool is registered on machine.

In this thread operator used "tip" but did not follow with selecting "in control" compensation which produced error in programmed path relative to how tool is registered at the machine.

Tools are touched so that high point of radius touches vertical or horizontal line which is in sink with two lines intersecting at 90 degree and that is the point we program.

I don't have Mastercam in front of me but I don't recall having to select tip at all, I select insert type and set radius, and few other parameters, selecting "in computer" compensation after that does all the magic.

There is also "left", "right" and "off", left and right are selected automatically based on tool type and orientation.

We really only need two kinds of tips, sharp point and tip tangent. Each of the two needs to be directly tied with 

"in control" and "in computer" compensation respectively.

So if I select "in computer" compensation, result should be pre calculated compensation and if I select "in control", code should have G41/G42/G40 and I need to finish the task at the machine.

In either case tools are touched at the machine same way regardless of angular differences of inserts.

Looking at tip choices in Fusion it is easy to misguide operator because it is not automated and needs coordinating with other settings, "center of insert" for instance is totally out of place because round insert can be programmed as any other insert using two methods described above.

So 1/4" round insert would have .125 radius and I can program using "in computer" or "in machine" compensation.

I worked in many shops and only 2 used "in control" compensation from 1995 on due to software being used to program work in computer on mass scale.

Operators no longer need to know how not to scrap parts with good programs because they entered wrong tip or no tip at all into machine offset page.

That's not to say that no one uses compensation at the machine via G41/G42, it's just so rare for many years now.

In one of the shops I had lead guy tell me that if I am not using G41/G42, I am not using compensation, and naturally ..... I laughed my **s off.

I can learn to work with software as it is built to work, just cannot let go of proven methods and definitions found in books written as guide to programming.

Because of clutter, lock of coordination and bugs in Fusion programming turning job in Mastrcam is a lot smoother and more intuitive for me, there are fewer bells and whistles to coordinate for desired result, at some point simplifying has to trim some of the fat but retain function.

[kretallick144]

Wow, ive open a can of worms.

Firstly, thankyou very much VicKosta for all your assistance!!  Alot of time gone into my issue,  very much appreciated.

So it all came down to tip compensation. I remember there use to be a pic in the tool setup showing it, but just a blank page now.

Your are correct in saying the tool description should have it covered.  Touch off for tool offset is the actual tool, not an imaginary line.

[Anonymous]

Cans of warms are all over forum, people asking for direction and others pointing them in both right and wrong directions.

I think we can all agree that passion with which we claim one thing or another drastically diminishes when we realize we are wrong due to overlooking something.

Running out of arguments to support the claim is "the moment of truth" but wars have been fought to the point of catastrophe in attempts to deny being wrong.

All books I opened in the past  talk about imaginary tool point in same context, one illustrated in figure showing insert radius touching horizontal and vertical lines intersecting each other at 90 degree.

This provides common denominator in the way tools are touched off at the machine and programmed.

If that's not so,............ question to be answered is,........... how would you coordinate 3 different imaginary points of tools having imaginary point relative to their angles , (35, 55 and 80 degrees) ?

What would I have to program as their commonly shared position that can be established at the machine ?

It seems to me each tool would have to be shifted by different amount in X and Z axis after physically touching them to same points on work piece,.................. and that is not how it works. 

[akash.kamoolkar]

FYI, @kretallick144 if you're getting lines in your NC code instead of arcs (the only issue i found with your part), you can fix it by going to the post process dialog and reducing the "built in minimum chord length" parameter until you get an arc.

Regards,

Akash Kamoolkar

[Anonymous]

Since "tip" ended up being the main issue in original post, I want to add few notes.

In following screen shots, pay attention to green point, that's the point of intersecting lines of insert geometry.

Note how it floats around based on insert radius, type and orientation?

Second thing to note is fact that all inserts have one common point regardless of orientation, geometry or radius value, that point is intersection of red lines representing axis and point commonly known as "imaginary point", the one used in coordination with "in computer" compensation and labeled as "tangent point" in Fusion.

With this illustration I have absolutely no idea what if any purpose "tip", as you define it, has in programming lathe work done in real world and in sink with programming manuals written for that purpose.

If it does anything, it confuses people trying to get grip on things but has no practical application and needs to be eliminated from list of "options", more is not better here.

[daniel_lyall · Accepted solution]

Thanks @akash.kamoolkar it is good to learn something new everyday.