Egg-Shaped Holes Revisited

[dxclark]

A recent post (http://www.emastercam.com/cgi-bin/ultimatebb.cgi?ubb=get_topic&f=1&t=000457) complained of egg-shaped holes. The general response suggested machine deficiencies as the most probable cause.

Please review the following code that mastercam puked out for me:

N10 O0000 (MC811-TEST )

N20 G0 G90 G80 G70 G40 G17

N30 T1 M6 ( 1/4 FLAT ENDMILL )

N40 G0 G90 S6000 M3 E1 X.215 Y0.

N50 G43 H1 D1 Z.25 M8

N60 Z.1

N70 G1 Z-.1 F6.

N80 G2 X-.2149 I-.215

N90 X.215 I.215

N100 G0 Z.25

N110 M5 M9

N120 T1 M6

N130 M30

Please note line #N80:

This is junk code on any machine!

I will try to ftp these files for further review.

MC811-TEST.MC8

MC811-TEST.NC

[Reece L Gibson]

Looks like a Fadal format? What is the tolerance of the machine for the start point and arc center before it alarms out? How are you measuring the hole roundness?

What was the measured results? We are talking a tenth here. depends on the geometry that was created, And if the post has been modified.

Alot of factors here to look at.

Looks like boring head teritory.

When I recreated this in MC8, it posted just fine.

[gstephens]

>N40 G0 G90 S6000 M3 E1 X.215 Y0.

.

.

>N80 G2 X-.2149 I-.215

>N90 X.215 I.215

.

.

>Please note line #N80:

>This is junk code on any machine!

Umm..I disagree. This code is perfect on almost any machine. Y0 is going to be modal and I or J = 0 should never need to be output. If the issue is with the .2149, apparently the arc center is not exactly at X0Y0, or the radius is .21495 or some such, and rounding inside the post is throwing off the I's and J's. There is no better output available unless you can program to 5 decimal places.

If you need tighter arc center tolerance, cut the part in metric (.001 mm = .000039 in)

[Charles Davis]

For your own peace of mind, just totally eliminate Mastercam as the problem.

Manually program a 1.0 diameter hole using one of the examples in the Fadal manual as a guide.

Put a dial indicator in the spindle and spin it. My guess is the hole will be elliptical. Time to call Service...

If the post is wrong, you might get an error at on the control, you may even skip part of the arc, but highly unlikely you'd ever get an oval.

[cadcam]

From my experience I am with Charles on this.

I to have come across this many a times.

[dxclark]

Thanks to all responents.

However, this is not a machine problem!

My machine makes perfectly acceptable circles when properly programmed to do so.

i.e. either 360 degree arcs or 2 - 180 degree arcs properly coded.

Please do not dismiss the .0001 error as insignificant until you have posted this to your machine.

Will any of you please send the faulty code I have described to your machine and describe the measured results.

I know you, like me , are too busy to tie-up a valuable machine tool and spend the time necessary to test this on a whim, but I am convinced (from actual practice) that the resultant part will be found unacceptable.

Thanks again.

[Guest]

Dxclark

I checked out your file. I analyzed the arc. The center of the arc is currently X.00004 Y0. When I posted it this way using the mpfan post I got the same result. But when I edited the arc center to be X0 Y0, the problem went away. Try changing the center of the arc and reposting. Good luck.

[dxclark]

mlindsey,

You're correct. The sample MC8 file was contrived like this intentionally to reflect a real-world condition that recently occurred.

My customers send solid models to me and I have to use them to create my tool paths. It is not practical (nor should it be necessary) to amend their geometry to accomodate mastercam.

[Luther_Heggs]

Increase your number of places behind the decimal point (screen cfg) and check the binary NCI from the Operation Manager dialog by the secret function on the dialog border and select OK.

[Luther_Heggs]

Secret command: hold down the Ctrl key and the Shift key while double-right clicking on the Operation Manager window outside of the tree control.

[dxclark]

LutherHeggs,

Please clarify:

Which item in screen config?

Which option in Secret-command?

[Reece L Gibson]

What do you call perfect round holes?

roundness with in .001, .0001,.00005?

in what material? or any material at all?

Ball bar test? is it 76 deg when you measure this hole?

[Charles Davis]

Wait a minute.... I've never known Mastercam to incorrectly round a number. If the last digit behind that displayed is 5 or greater, it rounds up. If less, it rounds down. That's how I'd do it too if I were writing the code by hand.

Basically, we're going to machine what the engineer draws. The databases are double precision, so there should be no roundoff errors in the data translation, or resulting from however we rotate, translate, etc.

Maybe I'm missing something here. Is there really some situation (once in a blue moon) that you can get into that you'd round otherwise because you know they intended an arc when but drew it "wrong"? Wouldn't this manifest itself in some other way, like a discontinuity between entities?

[ 08-06-2001: Message edited by: Charles Davis ]

[dxclark]

Millturn,

Sorry, I did not mean to imply that the circles are "perfect", only "perfectly acceptable".

i.e. within +/- .0005 on diameter in this instance. The actual error from my example produced an error approaching .005 dimensionally on my VMC.

Charles Davis,

A "rounding error" does not suggest an algorithmic error, but rather an error in fact!

The "rounded" portion of a number may have a deviation from the original number. This does produce a mathematical error. This error is evident in the sample code I provided.

[Charles Davis]

I talked about this with Marc Lindsey late this afternoon. I understand the problem more now. This is an odd one!

His idea was to truncate the number rather than round it; he's looking into it.

Another idea we had was to break the arcs into quadrants, rather than 180 degree arcs (yuk).

I THINK v9 will output 360 degree arcs.

[dxclark]

Charles Davis,

Thank you!

I was starting feel like "one against the world"! Although the sample I provided was contrived, to be sure, it was based on a customer's model. The "error" occurred twice in this one part. Once as a boss (like my example), and once as a hole.

I am not looking to find a "work-around". The program in question was already modified (by using 5 decimals of precision) and the parts were shipped.

I simply wanted to make public what I perceive as a flaw in this $**,*** program that I paid for.

Thanks again,

Dan

[Craig Madsen from CM3D]

I believe that if you add a J0 to the offending line (N80) you will solve your problem.

This is a common problem with many controls. They will 'fit' the arc to the endpoints unless forced to do otherwise.

To simulate what the control goes through, draw points at -.9999,0 and .9999,0 and then

create

arcs

endpoints

with a 1.0 inch radius, using the points.

When you analyze the arc center you will see a substantial error. This usually occurs with programs written using "R" values near 180 degrees. I will also occur if the control does not assume J0 for the unsupplied value.

I've been here before - for years.

Craig Madsen

[email protected]

[Toby]

Dxclark,

I also noticed that you have no lead in/out on that arc swing. Is there a reason for this? Have you tried adding the lead-ins and reposting?

[Wallace]

Hi Charles Davis,

For Mastercam around correcly:

Number of places in NCI = number of places in NC + 2 (or more).

If NCI = NC + 1; Mastercam not around.

This is definition the C++ not Mastercam.

But, Mastercam is write in C++.

Sorry my english...

Wallace M. Jr.

São Paulo - Brazil

[Surface]

I have experienced a simular problem which was easily solved by changeing the way the post outputs the arc. Many controls can accept arcs in diferent ways. It is my guess that the post outputs the information in an arc-rad format. The failsafe change is to change the output to an I,J format.

[Toby]

Surface,

Look at the code. It is I/J format.

Dxclark,

That comment "look what Masercam puked out for me" is just killing me.

[ 08-17-2001: Message edited by: toby ]

[Tony]

Hey there,

I have been down that egg shape hole road before .

In order for me to fix it ,I had to reset my controller's parameters from "Read circle from center point to read circle from endpoint" or vice versa...I forget.

I use in "Job setup" a seperate feed rate for arc's.

I am within .0005 good enough.....

[ 08-17-2001: Message edited by: Tony ]

[Guest CNC Apps Guy 1]

Toby,

I agree, that is hilarious. I didn't really look at it until you pointed it out. I never knoew Mastercam could puke. I wonder if I can get it to hurl something out, no, no, on second though that might not be such a good idea.