Surface high speed use?

[Darin]

Hello,

 

Lately I have been having bad issues with surface high speed .. I have scrapped three parts now ($20,000).. The more and more I look into the gouging issues the more and more I find that most people I talk to have stop using this because of these issues.. Why? Here are my settings .. The crash never comes up in backplot or verify.. We don't have Vericut or G code software .. But I sent the NC code to a friend who had Vericut and couldn't find it... How many people here have these issues? How many people here use high speed surface toolpaths? The main programmer here at one of the places I program for told me that there Mastercam dealer told him to only use old school flow line if you don't want to gouge part... I can send the nc code or file for people to test or look at.. I like the surface high speed because it makes programming easier.. I don't have to make 1000 separate surfaces for every feature so old school flow line will work.. Also I was told not to use solids for geometry that surfaces are safer... Is this all true? My boss wants to change to another cam software or program the old way with flow line.... I can't scrap another part here.. The crashes have been on a You-Ji VTL lathe with live tooling and Niigata horizontal machine.. The post are 8 to 10 years old.. But I was told this isn't the issue...

 

 

 

Thanks

[Newbeeee™]

If verify doesn't show and if more importantly vericut doesn't show....is it a machine parameter issue???

You can buy NCPlot very cheaply (a LOT less than $20k) - run it back through where the problem is on the part and look at the code. This will show if it is code or machine.

[Alien]

Hi,

I yesterday used this toolpath type and very very pleased with the result.

I am working on the HAAS vf 3 machine with TR160(5-axis).

I think that post 10 years old is a problem of crashing, because working in McamX7 with 10 years old post like driving Mercedes with wheel of a bicycle.

What can I suggest you is try the program with another post processor and compare NC files,

if you see difference in places where was crash - 100% problem in post and you need to update it.

If you don't see any collusion in backplot and verify, may be the machine set up (like reference point, retract height etc.) caused to crash.

I do not know how you do, I am always carefully running first part, directly from the machine, especially so expensive.

On the machine always possible to see where tool going, distance to go, etc.

Good luck!

Sincerely,

Michael.

[peon]

I have been using the HST's since their invention. I have only had gouges using the Hybrid toolpath. I did have better luck with surfaces in Versions 8, 9 and the first release of X, but since X2, I have been programming off of solids. If your buddy's reseller truly gave that advice, he should be shot and dumped in a ditch.

[Colin Gilchrist]

The first thing I would check would be the Arc settings in your Control Definition. The only time I've seen issues with gouging in a HST toolpath was due to the control reading a radius value, and swinging the wrong way around the arc.

 

Are you using IJK (Delta start-to-center) for your arc values, or are you using Radius? If your machine will accept it, please use the IJK option, as this specifies the exact arc centerpoint, and the machine doesn't have to guess.

 

The other clue here is the old posts as others have mentioned. We made some improvements around X4 or X5 in the posts for Arcs. Specifically, we added some code to force the internal calculations for the Arc centers to use the "Delta" values, even if you are outputting Radius for arcs.

 

Code:

# The following four initializations are used for full arc and helix arc output when the CD
#   is set to output R or signed R for arcs
larctypexz$  : 2	 #Lathe Arc center type XZ plane 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.
arctype$	 : 2	 #Mill Arc center type XY plane 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.
arctypexz$   : 2	 #Mill Arc center type XZ plane 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.
arctypeyz$   : 2	 #Mill Arc center type YZ plane 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.

 

If you don't see those 4 variable initializations in your post, then I would recommend you upgrade to a newer post processor. As a last resort, you can always turn off the arcs completely in the toolpath, and just go point-to-point moves (G1).

[peon]

After looking at your settings I noticed you are indeed using Hybrid. Turn off the horizontal arc on your leads page. Horizontal arcs have almost ALWAYS gouged on my parts using Hybrid. I have not had issues with the other HST's. I have not used Hybrid on X7, therefore I don't know if that issue was fixed or not, but I have abandoned that toolpath in X6.

 

 

Another tip: On your cut parameters page, change the "Keep tool down within" setting to a much smaller value. I prefer using the distance box rather than the tool percentage. I also noticed you are finishing with a .005" tolerance. THATS WAY TOO MUCH. I finish path with a tolerance between .0002"-.0004"

[Rstewart]

 

Another tip: On your cut parameters page, change the "Keep tool down within" setting to a much smaller value. I prefer using the distance box rather than the tool percentage. I also noticed you are finishing with a .005" tolerance. THATS WAY TOO MUCH. I finish path with a tolerance between .0002"-.0004"

 

 

^^^^^^

This. My worst finishing tolerance is .001" usually like .0005" I Work with solids about 90% of the time, there's Nothing wrong with them.

 

Just me, But I always opt for output feed move with the HS paths.

 

I too turn off the Horz arc on the lead in / off

[Oscar R.]

^^^^^^

This. My worst finishing tolerance is .001" usually like .0005" I Work with solids about 90% of the time, there's Nothing wrong with them.

 

Just me, But I always opt for output feed move with the HS paths.

 

I too turn off the Horz arc on the lead in / off

 

^^^^ Both of these ^^^^

 

I've used the solids as well, with no problems as far as toolpaths go. Processing or regen time can become a bit to much for my patience though.

 

I'll agree with tightening up the tolerance settings. I also have resorted to always using the output feed as this, I believe, is what caused a gouge in a program I did some time ago. And yes, it did NOT show in the verify.

 

I noticed you don't have your "Part Clearance" on at all. I would add some type of clearance and just because I like to be cautious, I'd also raise the "Clearance Plane" setting a bit.

[Jayson Kramer]

Solids and HST all the time . I have used them on allot of my customers parts all over the states and no issues.Well I have had one now that I think of it. but it was a fadal. it was the machine as I checked code and all was good .

[Chris Rizzo]

Can you post a pic of the gouge on the part? Is it a little gouge or huge arc-drive-the-wrong-way gouge? What machine control?Sounds like a machine/post issue though. I've wrecked some parts with arcs going the wrong way. Do what Colin says above. Also allow 360 deg arcs.

 

How big is the gouge? How big is the part? If the gouge is around .005, and your tolerance is set to that, then that's your cause. .005 may be perfectly fine if you've got that much tolerance, or on monster parts. But if not, that could be your cause.

 

Another GREAT tool for checking code is the full on version of Cimco V6. It's very inexpensive and worth it's weight in gold.

 

. ....Reseller for Wash?

[Darin]

Thanks guys for the honest feed back on this... I think I am going to start with a new post and go from there... Here is a picture of the gouge ... The You-Ji's have Fanuc 18i-TB and Oi-TC controls...

[Darin]

^^^^^^

This. My worst finishing tolerance is .001" usually like .0005" I Work with solids about 90% of the time, there's Nothing wrong with them.

 

Just me, But I always opt for output feed move with the HS paths.

 

I too turn off the Horz arc on the lead in / off

 

 

When you say Horz arc on lead in/off you mean this page and put 0 to turn off? I don't see an off...

[Darin]

The first thing I would check would be the Arc settings in your Control Definition. The only time I've seen issues with gouging in a HST toolpath was due to the control reading a radius value, and swinging the wrong way around the arc.

 

Are you using IJK (Delta start-to-center) for your arc values, or are you using Radius? If your machine will accept it, please use the IJK option, as this specifies the exact arc centerpoint, and the machine doesn't have to guess.

 

The other clue here is the old posts as others have mentioned. We made some improvements around X4 or X5 in the posts for Arcs. Specifically, we added some code to force the internal calculations for the Arc centers to use the "Delta" values, even if you are outputting Radius for arcs.

 

Code:

# The following four initializations are used for full arc and helix arc output when the CD
# is set to output R or signed R for arcs
larctypexz$ : 2	 #Lathe Arc center type XZ plane 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.
arctype$	 : 2	 #Mill Arc center type XY plane 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.
arctypexz$ : 2	 #Mill Arc center type XZ plane 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.
arctypeyz$ : 2	 #Mill Arc center type YZ plane 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.

 

If you don't see those 4 variable initializations in your post, then I would recommend you upgrade to a newer post processor. As a last resort, you can always turn off the arcs completely in the toolpath, and just go point-to-point moves (G1).

 

 

Thanks Colin again for your help.... Here is the post.. I don't find those exact lines like the one above.. Also a screen shot of the control settings...

 

 

 

 

 

[post_VERSION] #DO NOT MOVE OR ALTER THIS LINE# V15.00 P2 E1 W15.00 T1337895755 M15.00 I0 O0

# Post Name : YOU JI

# Product : LATHE

# Machine Name : YOU JI

# Control Name : OI

# Description : YOU JI C-AXIS POST

# Mill/Turn : YES

# 4-axis/Axis subs. : YES

# 5-axis : NO

# Subprograms : YES

# Canned Cycles : YES

# Executable : MP 10.0

#

# WARNING: THIS POST IS GENERIC AND IS INTENDED FOR MODIFICATION TO

# THE MACHINE TOOL REQUIREMENTS AND PERSONAL PREFERENCE.

#

# Associated File List$

#

# GENERIC FANUC 4X MT_LATHE.control

#

# Associated File List$

#

# --------------------------------------------------------------------------

# Revision log:

# --------------------------------------------------------------------------

# Programmers Note:

# CNC 07/7/04 - Initial post update for Mastercam X

# DV 05/03/13 - Modified R output for drilling, and Coordinate conversion

#

#

# --------------------------------------------------------------------------

# Features:

# --------------------------------------------------------------------------

####### MILL/TURN FUNCTIONS SUPPORTED BY THIS POST #######

#

# This post supports Generic Fanuc code output for mill/turn lathes.

# It is designed to support the features of Mastercam X.

#

## NEW FEATURES FOR X

# - Machine definition, control definition and toolpath group parameter read sections added.

# - Variable initialization with CD_VAR are read directly from CD. Changing these initial values

# in the post will not effect output. These values are only processed during the update post routine.

# - Variable initialization with SET_BY_MD or SET_BY_CD are overwritten in this post by parameter or

# variable settings from MD or CD.

# - Enhanced tool information - Added switch for tool comments (see tool_info)

# - Supports X comments including machine name, group name and group comment output (see pcomment2)

# - Additional date, time and data path output options (see pheader)

# - Support for 10 additional canned text options for X

# - Decimal support for sequence number output (set "Increment sequence number" in CD to a decimal value

# for output. I.E. "Increment sequence number" = .5, "Start sequence number" = 10 : N10, N10.5, N11, N11.5, etc...)

# - Switch for output of M00 or M01 at tool change (3 position switch, off, M00, M01 - see prog_stop)

# - Support for seperate XY, XZ and YZ plane/arc variables (see Arc page in CD)

# - Support for X style coolant. Allows up to 10 different coolants to be turned on/off before, with, or after like

# canned text. Coolant output is handled by "coolant" variable and string selector for V9 style coolant,

# "coolantx" variable and string selector for X style coolant.

#

# Following Misc. Integers are used:

#

# mi1 - Work coordinate system: (home_type)

# -1 = Reference return / Tool offset positioning.

# 0 = G50 with the X and Z home positions.

# 1 = X and Z home positions.

# 2 = WCS of G54, G55.... based on Mastercam settings.

#

# mi2 - Absolute or Incremental positioning at top level

# 0 = absolute

# 1 = incremental

#

# mi3 - Select G28 or G30 reference point return:

# 0 = G28, 1 = G30

#

# mi4 - Canned conversion cycle type selection:

# Mill-

# Activates milling axis conversation canned cycles (G107 or G112).

 

 

 

 

 

 

parc #Select the arc output

#Setup for arctype setting

if (posttype$ = 2 & (larctypexz$ = one | larctypexz$ = four)) |

(posttype$ = 1 &(plane$ = zero & (arctype$ = one | arctype$ = four)) | #XY Plane

(plane$ = one & (arctypeyz$ = one | arctypeyz$ = four)) | #YZ Plane

(plane$ = two & (arctypexz$ = one | arctypexz$ = four))), #XZ Plane

[

result = newfs(two, i$)

result = newfs(two, j$)

result = newfs(two, k$)

result = newfs(two, iout)

result = newfs(two, jout)

result = newfs(two, kout)

]

else,

[

result = newfs(three, i$)

result = newfs(three, j$)

result = newfs(three, k$)

result = newfs(three, iout)

result = newfs(three, jout)

result = newfs(three, kout)

]

if (posttype$ = 2 & (plane$ = 2 & larctypexz$ < five)) |

(posttype$ = 1 & ((plane$ = 0 & arctype$ < five) |

(plane$ = 1 & arctypeyz$ < five) |

(plane$ = 2 & arctypexz$ < five))),

[

#Arc output for IJK

if (posttype$ = 2 & (plane$ = 2 & larctypexz$ = one)) | #XZ plane - Lathe

(posttype$ = 1 & ((plane$ = zero & arctype$ = one) | #XY Plane - Mill

(plane$ = one & arctypeyz$ = one) | #YZ Plane - Mill

(plane$ = two & arctypexz$ = one))), #XZ Plane - Mill

[

#Arc output for IJK, absolute

iout = (iout + dia_shift) * dia_mult

jout = (jout + y_shift) * y_mult

kout = (kout + z_shift) * z_mult

if c_ax_flp, iout = -iout

]

else,

[

#Arc output for IJK, start/center

iout = iout * (dia_mult/abs(dia_mult))

jout = jout * y_mult

kout = kout * z_mult

if c_ax_flp, iout = -iout

]

iout, kout, jout

!i$, !j$, !k$

]

else,

[

#Arc output for R

if abs(sweep$)<=180 |

(posttype$ = 2 & (plane$ = 2 & larctypexz$ = five)) | #XZ Plane - Lathe

(posttype$ = 1 & ((plane$ = 0 & arctype$ = five) | #XY Plane - Mill

(plane$ = 1 & arctypeyz$ = five) | #YZ Plane - Mill

(plane$ = 2 & arctypexz$ = five))), result = nwadrs(srad, arcrad$) #XZ Plane - Mill

else, result = nwadrs(srminus, arcrad$)

*arcrad$

]

pffr #Output feedrate, force

if ipr_actv$ = zero, pfr_m

else, pfr_l

*feed

pfr #Output feedrate

if ipr_actv$ = zero, pfr_m

else, pfr_l

`feed

pfr_m #Format feedrate for mill

result = nwadrs(strf, feed)

result = newfs (17, feed)

pfr_l #Format feedrate for lathe

if opcode$ = 104,

[Darin]

^^^^ Both of these ^^^^

 

I've used the solids as well, with no problems as far as toolpaths go. Processing or regen time can become a bit to much for my patience though.

 

I'll agree with tightening up the tolerance settings. I also have resorted to always using the output feed as this, I believe, is what caused a gouge in a program I did some time ago. And yes, it did NOT show in the verify.

 

I noticed you don't have your "Part Clearance" on at all. I would add some type of clearance and just because I like to be cautious, I'd also raise the "Clearance Plane" setting a bit.

 

For some reason the part clearance doesn't work with full vertical retract... It is grayed out... I was told to use full vertical retract it is safer...

 

 

Thanks

[Colin Gilchrist]

From what others in the thread have said, I'm leaning towards the Hybrid arcs being the culprit, not the post itself. Those CD settings look spot on, so your problem is likely not the arc settings in the NC code.

 

Tolerance also has a lot to do with it. For finishing, I typically go 2:1 ratio, with .0003 total tolerance.

[Darin]

From what others in the thread have said, I'm leaning towards the Hybrid arcs being the culprit, not the post itself. Those CD settings look spot on, so your problem is likely not the arc settings in the NC code.

 

Tolerance also has a lot to do with it. For finishing, I typically go 2:1 ratio, with .0003 total tolerance.

 

Ok thanks Colin... So I should never use Hybrid? Also should I always have the total tolerance 2:1 even if I am roughing? Could the total tolerance settings have made this gouge?

 

 

Thanks

[Darin]

Can you post a pic of the gouge on the part? Is it a little gouge or huge arc-drive-the-wrong-way gouge? What machine control?Sounds like a machine/post issue though. I've wrecked some parts with arcs going the wrong way. Do what Colin says above. Also allow 360 deg arcs.

 

How big is the gouge? How big is the part? If the gouge is around .005, and your tolerance is set to that, then that's your cause. .005 may be perfectly fine if you've got that much tolerance, or on monster parts. But if not, that could be your cause.

 

Another GREAT tool for checking code is the full on version of Cimco V6. It's very inexpensive and worth it's weight in gold.

 

. ....Reseller for Wash?

 

 

Hi Chris... Thanks for the input.. I am assuming the person meant Oregon reseller but not sure.. It is one of the many place I program for . I hear a lot of feedback from different people so I take a lot of the things I hear with a grain of salt.. I can only go from my experience on the hundred's of machine I have dealt with.. I haven't see these tool paths do this till now.. I am glad I have some great contacts like yourself and others... I have some that actually have You-Ji's running with Mastercams and they don't have these issues... So it is a lot of investigating that I have to do... It might be a simple as getting the control settings right on the machines....

 

Thanks

[Colin Gilchrist]

Ok thanks Colin... So I should never use Hybrid? Also should I always have the total tolerance 2:1 even if I am roughing? Could the total tolerance settings have made this gouge?

 

 

Thanks

 

Hi Darin,

 

No, I'm not saying you need to never use Hybrid. I'm saying you should set the Horizontal Arcs setting to zero for the linking parameters. That should prevent the issue from showing up in X6. This issue has been fixed in X7, and all linking moves are now gouge checked against the drive and check surfaces. (BTW, X7 also now supports check surfaces for these HST toolpaths)

 

I prefer the 2:1 ratio when setting my filter, as it keeps the path more accurate, while allowing better arc filtering. You can do a search on this forum for information about the toolpath filter and find some great info. There are basically two filters that run when you make a toolpath. First, the entire path is linearized, using the 'cut tolerance'. This is a bi-lateral tolerance that determines the initial accuracy of your toolpath. After the cut tolerance filter runs, then the Arc Filter is run. This filter will fit an arc to the linear segments, within the given tolerance.

 

My basic starting parameters for Total Tolerance is 10% of the Stock to Leave value. So if you are leaving .100 of stock on your surfaces, then using .009 for the total tolerance is a good value. The larger the tolerance, the more filtered your code is.

 

For finishing, I like to use a value of .0003 for most contouring/surfacing. The only exception for me is very tight tolerance cuts. In that case I will go down to .00001 or less for my total tolerance, basically whatever the lowest tolerance the dialog will let me enter.

 

The ratios you choose just take the total tolerance and divide that value up between the two different filters according to the ratio you select or enter.

 

Hope that helps,

 

Colin

[baldhead]

1. Could this be a dog leg rapid move below Z zero? On some machines a dog leg rapid shows up as a strait line move in verify. I had this problem with verify because my machine moves in dog leg rapid. Everything looks good but your machine does not rapid as shown in verify.
   

[Redfire427]

The most glaring error I see in your settings is that you have the "rapid retracts" button checked. You should never use rapid moves in a high-speed tool path. Mastercam does not check for dog-leg moves, and it is these "dog-legs" that WILL cause a crash or gouge. You should uncheck the box and use a high feedrate. This will force the output to a linear move.

 

Carmen

[Newbeeee™]

1. Could this be a dog leg rapid move below Z zero? On some machines a dog leg rapid shows up as a strait line move in verify. I had this problem with verify because my machine moves in dog leg rapid. Everything looks good but your machine does not rapid as shown in verify.
   

 

Irrespective of whether the settings for arc/lead in are correct or not, verify still didn't show the gouge and vericut also didn't show the gouge.

So my money is on either the above (dogleg) or IJK/rad problem with the machine controller.

[Mike Whitten CAD/CAM Contractors]

The image looks like an arc reversal or similar. I have had this issue one time with an HST path(not Hybrid) and also junked out a very expensive part. We were lucky and it was welded. I worked on this issue for quite a while at a customers facility and found that someone had just recently changed the IJK arc setting in the post (CD) to break at 90. This was a perfect proven post before the edit. Once is was changed back to break at 180, the issue was gone.

 

Machine: newer Mori NH8000 HMC

post: 2008 ish mpmaster

MC version: X6 mu2

 

I checked the code in Predator VCNC and NCPlot and it looked perfect in both softwares. The path was inches off at the machine.

 

I have never seen this issue except this one time. I would do as suggested, and use a newer post. I am thinking that a high-end package like Vericut could find something like this, but I do not own it.

 

Thanks,

[Rotary Ninja]

^^^ Good Advice

[TK-32™]

I linearize all arcs and use Advanced Look Ahead {G05.1Q1, (ON) G05.1, Q0(OFF)} on two of our FANUCS because we had the same problems. I haven't had a gouge ever since.

Well, I have had some but those were my mistakes.

[mkd]

The image looks like an arc reversal or similar. I have had this issue one time with an HST path(not Hybrid) and also junked out a very expensive part. We were lucky and it was welded. I worked on this issue for quite a while at a customers facility and found that someone had just recently changed the IJK arc setting in the post (CD) to break at 90. This was a perfect proven post before the edit. Once is was changed back to break at 180, the issue was gone.

 

Machine: newer Mori NH8000 HMC

post: 2008 ish mpmaster

MC version: X6 mu2

 

I checked the code in Predator VCNC and NCPlot and it looked perfect in both softwares. The path was inches off at the machine.

 

I have never seen this issue except this one time. I would do as suggested, and use a newer post. I am thinking that a high-end package like Vericut could find something like this, but I do not own it.

 

Thanks,

I had the exact same experience with MC9, IJK arcs broken at 90 on a mori Horz.

postmortem through a friend's vericut showed good code.

changed to Rs for that machine and it ran fine.