Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Forcing arcs into line segments for better accuracy?


Recommended Posts

The component I am working on has an overall profile tolerance of .005 to the entire model. There are dozens of small internal corners, all normal 90 deg arcs. Most of these arcs are falling out of tolerance on the .005 profile.

I am already using a smaller endmill than the radius size of the arcs to reduce tool contact, and running modest feed rates and spring passes. 

I was recommended by a programming consultant to try turning on my machine's high speed look ahead funtions (Matsuura MX 520) and also to break all the arcs into line segments with smoothing settings in order to achieve better accuracy. Does anyone have experience with this type of strategy?

Link to comment
Share on other sites

Your High Speed look ahead settings are not being set or not tuned correctly if you have arcs in the toolpath. Can have 1 trillion points on a arc and get 1 trillion lines of code, but when a machine will not machine an arc correctly when told to do so then the highspeed look ahead setting are either not set correctly or not being used correctly. I have seen both issues on machines, but I have cut .0002" profile parts on those machines with no issues using arcs so have to think your not using them correctly. What settings are you using in the fine cutting setting when using them? 

Calling CNCAPPS guy. Calling CNCAPPS guy.

He knows the machine very well and hopefully will be chiming in soon. If not I will text him and ask him to chime in.

  • Like 1
Link to comment
Share on other sites

I should mention, I have added BOTH high speed look ahead and broken the arcs into segments now. My initial toolpaths when the arcs were out of tolerance were NOT using HSM settings, and each arc was just one line of code G2/G3. 

 

Also I should mention these are not 3d features, just plain 2d vertical internal corners. 

Link to comment
Share on other sites

Couple of quick thoughts.

Is it undercutting, or over-cutting in the corners?  I am assuming that the spring passes would be taking care of a stock plus situation, but sometimes given the tool setup, even with a few spring passes you can still get tool deflection depending on length of cut.  I would think the stock high speed settings in the machine would be pretty good, so let's talk about the cut itself first and eliminate that as the cause before we dig into look-a-head.  What type of holder, stick-out/projection, and cutter(# flutes, helix angle for starters),  do you have?  Also, what material are you cutting?  Feeds, speeds, radial and axial depth of cut?

Link to comment
Share on other sites
20 minutes ago, huskermcdoogle said:

Couple of quick thoughts.

Is it undercutting, or over-cutting in the corners?  I am assuming that the spring passes would be taking care of a stock plus situation, but sometimes given the tool setup, even with a few spring passes you can still get tool deflection depending on length of cut.  I would think the stock high speed settings in the machine would be pretty good, so let's talk about the cut itself first and eliminate that as the cause before we dig into look-a-head.  What type of holder, stick-out/projection, and cutter(# flutes, helix angle for starters),  do you have?  Also, what material are you cutting?  Feeds, speeds, radial and axial depth of cut?

Yes I agree if you leaving .05 stock for a .031 endmill and trying to cut 2" deep no settings in the world will overcome that as bad machining process. Don't laugh I have seen it tried.

  • Like 1
Link to comment
Share on other sites
47 minutes ago, huskermcdoogle said:

Couple of quick thoughts.

Is it undercutting, or over-cutting in the corners?  I am assuming that the spring passes would be taking care of a stock plus situation, but sometimes given the tool setup, even with a few spring passes you can still get tool deflection depending on length of cut.  I would think the stock high speed settings in the machine would be pretty good, so let's talk about the cut itself first and eliminate that as the cause before we dig into look-a-head.  What type of holder, stick-out/projection, and cutter(# flutes, helix angle for starters),  do you have?  Also, what material are you cutting?  Feeds, speeds, radial and axial depth of cut?

The pre-finishing toolpath is an optirough leaving .0065 on the walls.

internal corners are being left material heavy

6061 alum, the part internal corners are Ø.1875 and I am using a Ø.1562 X .750 loc 38° 3 flute endmill, in a Nikken SK16 X 90mm gage holder, 6000 Rpm 20 ipm feed. The deepest of these corners is about .500 depth tool engagement. 

Again, the initial toolpaths did not have ANY look ahead functions on.

If it were any other situation than a .005 profile tolerance, it would be fine, but these corners are out by about .0005-.002

Link to comment
Share on other sites
2 hours ago, machineimpossible said:

The pre-finishing toolpath is an optirough leaving .0065 on the walls.

internal corners are being left material heavy

6061 alum, the part internal corners are Ø.1875 and I am using a Ø.1562 X .750 loc 38° 3 flute endmill, in a Nikken SK16 X 90mm gage holder, 6000 Rpm 20 ipm feed. The deepest of these corners is about .500 depth tool engagement. 

Again, the initial toolpaths did not have ANY look ahead functions on.

If it were any other situation than a .005 profile tolerance, it would be fine, but these corners are out by about .0005-.002

Too much load on that tool. Take a spring pass in the corner using the same speeds and feeds and your part will come into tolerance. All tools move and that tool is deflecting. Want to test my call take a .00005" indicator and run it up and down the corner and see the taper you're getting from top to bottom. I watched a 1/4 ball endmill deflect to almost 30 degrees one time and not break.

I was machining a locate slot on a 40 ton turbine housing about 25 years ago on a HBM. 3 other people had tried all of them with 20+ years experience and they all failed. The slot was 6" deep and had to have a .001 tolerance from top to bottom. I took the 2" diameter 6 flute endmill and worked on it for 6 hours. I had 4 different indicators setup to control back lash. I took 12 cuts in the same place and all 12 cuts removed material. It wasn't until the 12 cut that I got the doblocks to go from top to bottom on that shape. Why was that? Tool deflection.

The .0065 of material for 1/2" of of material is a lot of material to remove for a finish pass. Try getting a 7 flute endmill and take the same cut the difference will be night and day. Lets teach you some Physics about tools. The cross section of 3 flute tool is about 45-50% of the tool diameter. That means your tool effective strength ratio to length of cut is at 50% of the tool diameter. Your working with .08 diam of tool to fight against push back from the material as it is cutting. Now you have .0065 of material and that is about 8.5% of the effective tool diameter fighting against you to do this with. Now move to a 7 flute tool and you have about 70-75% off the tool diameter to work with. You have a much stronger tool due to the core being a bigger diameter. People always think you must use a 3 flute tool when finishing aluminum. No you don't have to use a 3 flute tool to finish aluminum. I will use a uncoated 5-7 flute tool in aluminum all day long with superior results to a 3 flute tool. Problem is finding them uncoated. Problem is the aluminum will stick to any tool costed with an aluminum substrate and that is the bigger issue doing it than the tool loading up for finishing.

  • Like 1
  • Huh? 2
Link to comment
Share on other sites

My suggestion would be to helix interpolate your corners then do your finish passes, or do your it in two depth cuts with a spring at each level. 

I agree that tool deflection is likely the culprit.  That is a way bendy tool.  You are at 5xØ if you were to bury the tool up to the flutes, but in reality you are probably at close to 6xØ.  I am guessing .850 stickout?  You would likely be good if you were at 3xØ or less.

As Ron mentioned, take an indicator and check the wall deflection.  I would expect on a straight portion with a spring pass you probably have .001" or so.  Once the engagement goes up as it will in the corner, you will have much much more.  By my math assuming 45 degree helix, you have a pretty even split of 3 and 4 points of contact in cut when you go through the corners.  In a straight wall situation, you still have a mixture of 3 and 4 contact points, but more on the 3 side.  With less depth of cut you would be in the 1 to 2 contact point, not ideal, might chatter, but won't deflect nearly as much (less than half).

All that said, there is also no reason you should not max out your spindle speed to 12000, you could also probably double your chip load and still be conservative.  12k @ 50ipm should be good for a new starting place.  Reduce feeds by 50% in the corners.  With increase in speeds and feeds you should get it done in the same amount of time.  With that machine you should be able to hold very tight tolerances at 50ipm.  Much tighter than you are likely seeing for cutter deflection.

  • Like 4
Link to comment
Share on other sites

In those cases i have had really great luck kicking the part at an angle and using a ball em to surface the corner. Yes it does take longer but given you have a machine that has 5x capabilities and it is really tight (center of rotation is dialed in ) then it works great. Blending two tools isn't ideal but again, if the machine is tight then it's no issue. 

Also have used a ball em of equal radius as the part fillet and used multiaxis morph  to drive the tool using 1 pass (determined by number of cuts, area type) That is my preferred method because the surface  finish is beautiful especially in aluminum.

Only using 3 axis is preferred but if the machine is tight then use the features you paid for. 

  • Like 3
Link to comment
Share on other sites

On your Matsuura you want to ALWAYS use the High Speed Modes. Make sure to use the correct High Speed Mode for the type of machining.

2D = G131P...

3D = G131M...

Rotary =G131 F...

Canned Cycles = G131 D1

In each mode (other than drilling) there are 3 settings.

1=Roughing/General machining

2=Semi-Finish/Finish

3=Fine Finish. 

Or 1=Speed Preference to 3= Accuracy Preference.

You should be able to hold single digit micron accuracy on a 2D profile using G131P3 with arcs  (provided the CAD is good) or line segments. 

Are you using CAMplete?

  • Like 6
Link to comment
Share on other sites
1 hour ago, cncappsjames said:

On your Matsuura you want to ALWAYS use the High Speed Modes. Make sure to use the correct High Speed Mode for the type of machining.

2D = G131P...

3D = G131M...

Rotary =G131 F...

Canned Cycles = G131 D1

In each mode (other than drilling) there are 3 settings.

1=Roughing/General machining

2=Semi-Finish/Finish

3=Fine Finish. 

Or 1=Speed Preference to 3= Accuracy Preference.

You should be able to hold single digit micron accuracy on a 2D profile using G131P3 with arcs  (provided the CAD is good) or line segments. 

Are you using CAMplete?

So I just did a cycle with all the 2d contours with the arcs set to about .0008 line segments and using G131 R10, would the P3 setting be better than R10? As I understand it from the manual G131 R1-10 will function the same as FANUC G05.1? 

waiting to get a report from CMM monday. 

We are using camplete for verification, but not running code from Camplete, as the machine is missing functions that Camplete post uses. Its a long story, but basically when the machine was purchased around 2011, they declined on just about every controller option. As such, the machine has no TWP (G68.1) no WSEC, no data server memory (only as 3000kb) no additional offsets, absolute bare bones controller. About the only option that it has which all 5 axis should have is TCP

 

Link to comment
Share on other sites
8 minutes ago, machineimpossible said:

So I just did a cycle with all the 2d contours with the arcs set to about .0008 line segments and using G131 R10, would the P3 setting be better than R10? As I understand it from the manual G131 R1-10 will function the same as FANUC G05.1? 

waiting to get a report from CMM monday. 

We are using camplete for verification, but not running code from Camplete, as the machine is missing functions that Camplete post uses. Its a long story, but basically when the machine was purchased around 2011, they declined on just about every controller option. As such, the machine has no TWP (G68.1) no WSEC, no data server memory (only as 3000kb) no additional offsets, absolute bare bones controller. About the only option that it has which all 5 axis should have is TCP

 

Amazing people cheap on the important stuff then wonder why your fighting to make good parts. I understand the user name now. Best of luck getting it sorted out.

  • Like 1
Link to comment
Share on other sites

My condolences @machineimpossible.  An NC Format can be configured to take advantage of what you do have. PM me and I can help you get that sorted out. CAMplete is a vital tool IMHO.

So, the R-level modes are old school. Not tailored for they type of machining at hand.

By using only G05.1 you would be missing out.

By using R levels you are missing out. With R, you only have 11 settings period. (R0 through R10) By using P, M or F when combined with the sliders, each mode has 10 possible settings, for a total of 31 setting possibilities.

So if you set G131R3, then move the slider all the way to the right, this will give you max precision, activate any and all control contour control functions available on the machine, plus allow you to run arcs for smaller programs.

Do this;

Poor Man's Dataserver.

https://www.dropbox.com/s/wkro1ylu2im5ir5/M198 to Flash Card Procedure - FANUC 30i-31i Updated.pdf?dl=0

 

Hope this helps. 

  • Like 3
Link to comment
Share on other sites
11 minutes ago, cncappsjames said:

My condolences @machineimpossible.  An NC Format can be configured to take advantage of what you do have. PM me and I can help you get that sorted out. CAMplete is a vital tool IMHO.

So, the R-level modes are old school. Not tailored for they type of machining at hand.

By using only G05.1 you would be missing out.

By using R levels you are missing out. With R, you only have 11 settings period. (R0 through R10) By using P, M or F when combined with the sliders, each mode has 10 possible settings, for a total of 31 setting possibilities.

So if you set G131R3, then move the slider all the way to the right, this will give you max precision, activate any and all control contour control functions available on the machine, plus allow you to run arcs for smaller programs.

Do this;

Poor Man's Dataserver.

https://www.dropbox.com/s/wkro1ylu2im5ir5/M198 to Flash Card Procedure - FANUC 30i-31i Updated.pdf?dl=0

 

Hope this helps. 

Why you were called when I saw the machine. Thank you as always sir for chiming in and sharing your knowledge to help others.

  • Like 1
Link to comment
Share on other sites

The g131 doesn't work unless you have the g05.1 on.

 

We turn on 1604 bit 0 so it is on automatically. Then just worry about g131.

The r values still work.

With P M and f there are three separate tables to get the looked ahead parameters from so you could customize them. But they're pretty much all the same from the factory.

 

I believe our machine came with two NC formats and one of them was a standard five axis with no TWP or G 43.4

  • Like 1
Link to comment
Share on other sites
4 hours ago, Leon82 said:

its the same with our vplus 1000.

I have NEVER activated G05.1 prior to activating G131. Not once.

In nearly 15 years as an AE supporting the line, through all my training, factory or otherwise not once have I heard that was suggested or even necessary. So who said that was necessary? You can PM me if you don't want to say publicly.

Link to comment
Share on other sites

Circle milling a 1.375 dia for a ball lock was my first time on an mx. Hole was .01 undersize.at 130 ipm. As soon as g5.1 was activated and r10 selected it came within .001.(most enddmills are undersized}.

 

Once I changed parameter 1604 bit 0 to 1 g131 works as needed. 1604 but 1 turns aicc mode on by default.

 

On the vplus my chamfer at 40 ipm was making a rounded corner. I tried g5.1 and it worked as desired so I changed 1604 bit 0 to 1 and it's been fine ever since.

I tried it myself I never really asked anybody.

I'm convinced at the factory they spin a parameter wheel And whatever it lands on they load. So maybe yours don't need it I'm not sure

  • Like 1
Link to comment
Share on other sites

Here's the factory parameter group for #1604 for all 5-Axis machines I've put my hands on.

N01604Q1L1P00000000

Here's my ballbar test program; (Uses G131 P3 only)

I never use R unless that's all the machine has. Using R doesn't take advantage of tuning for specific types of machining.

%
<XY_150MM_BALLBAR>(MC 214)
 
(212: XY 360deg 150mm Calibrated)
(XY, 360 degree test, 5.906 in radius, 196.85 in/min feedrate)
(Work offset must be defined where the centre mount is positioned)
 
N10G20(input in in)
N20G54.1P300(set origin position)
N30G90(absolute dimensions)
N40G17(XY plane)
N50G64(disable stopping between moves)
N60M19
N70M05
N80G131P3
N90#3006=1(INSTALL MAG BASE SETTING CUP ON CENTER OF TABLE)
N100#3006=2(CALL AN UNUSED TOOL TO THE SPINDLE)
N110#3006=3(INSTALL MAGNETIC TOOL CUP AND CUP EXTENSION IN TOOL HOLDER)
N120#3006=4(JOG HOLDER AND HANDLED SETTING BALL TO MAGNETIC BASE SETTING CUP)
N130#3006=5(HANDLED SETTING BALL MUST MOVE FREELY AND BE IN CONTACT WITH BOTH SETTING CUPS)
N140#3006=6(MOVE LEVER ON MAGNETIC BASE SETTING CUP TO LOCK INTO POSITION)
N150G90G10L20P300X#5021Y#5022Z#5023B0.C0.
N160G11
N170#3006=7(JOG SPINDLE AWAY AND REMOVE HANDLED SETTING BALL AND STORE)
N180#3006=8(DID YOU DO IT ALL?)
N190#3006=9(ARE YOU SURE?)
N200G94F196.85(feedrate in in/min)
N210G01X-5.965Y0.000Z0.000(move to start point)
N220M00(stop to load ballbar)
N230G01X-5.9055Y0.000(in feed)
N240G03X-5.9055Y0.000I5.9055J0.000(CCW arc)
N250G03X-5.9055Y0.000I5.9055J0.000(CCW arc)
N260G01X-5.965Y0.000(out feed)
N270G04X1.(pause between runs)
N280G01X-5.9055Y0.000(in feed)
N290G02X-5.9055Y0.000I5.9055J0.000(CW arc)
N300G02X-5.9055Y0.000I5.9055J0.000(CW arc)
N310G01X-5.965Y0.000(out feed)
G130
N320M30(end of program)
%

 

5000mm/min feed - 150MM Rad.

.005mm is the usual deviation on the test.

G131P3 only.

I mean if it works for you, I guess it's fine.

Link to comment
Share on other sites
15 hours ago, cncappsjames said:

5000mm/min feed - 150MM Rad.

.005mm is the usual deviation on the test.

G131P3 only.

I mean if it works for you, I guess it's fine.

Will the machine feed that fast in P3?  I recall P3 level putting a pretty aggressive cap on my feedrates.

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...