Problem with surface quality

[JFGuffie]

Hello

I'm programming and running an impeller on a new Integrex 250 with Smooth.. 

I have some issues with getting nice surface quality.. I have tried many setting, spoken with my Mastercam reseller as well as Mazak for finding optimal parameters etc.. 

The weird thing is that I get a better surface with more rough filter and cut tolerance, compared to when I choose to remove filter and go with very narrow cut tolerance.. But both of them doesn't give me what I expected.. 

I have attached my program as well as a picture of a finished wing.. The upper part is done with fine cuttingt tolerance and no filter.. The lower part is done with more rough tolerance and filter as well..

The red arrow just refer to a finish, where I have move the tool 0.01 to ensure it wasn't tool deflection that caused the problem..

Can anyone help to guide me in which direction to go, maybe different type of toolpath or something to get a better surface finish?

Thanks

Impeller.mcam

[rgrin]

I don't have a millturn environment, but I am able to backplot your toolpath it seems.  Any particular reason you're using a bullnose endmill as opposed to a ball endmill? Traditionally I have seen people finishing the blades with a taper necked ball and the current hotness is the fancy form cutters.

Another thing too is it looks like you're feeding the tool at 3000mm/min? That converts to like 120 inches per minute for my American brain.  That seems awfully quick, especially since it looks like you are zigzagging. I would say the toolpath look fairly normal other than the quirky retracts at the edge of the blade on the first paths. I would personally try and get the toolpath to wrap around the blade in 1 motion so that way you are climb cutting the whole way down. 

Switching to a ball will give you a larger radius you're cutting on and give you fewer scallops than your bull nose. I would personally use the toolpath with the most points and then mess with any smoothing settings on the cnc control to get the finish I want.

[#Rekd™]

+1 to using a ball nose end mill.

 

Also you can try using "Angle Increment" in Tool Axis control to make the vectors closer together (using a small number like 0.5 degrees or smaller)

[JFGuffie]

8 minutes ago, rgrin said:

I don't have a millturn environment, but I am able to backplot your toolpath it seems.  Any particular reason you're using a bullnose endmill as opposed to a ball endmill? Traditionally I have seen people finishing the blades with a taper necked ball and the current hotness is the fancy form cutters.

Another thing too is it looks like you're feeding the tool at 3000mm/min? That converts to like 120 inches per minute for my American brain.  That seems awfully quick, especially since it looks like you are zigzagging. I would say the toolpath look fairly normal other than the quirky retracts at the edge of the blade on the first paths. I would personally try and get the toolpath to wrap around the blade in 1 motion so that way you are climb cutting the whole way down. 

Switching to a ball will give you a larger radius you're cutting on and give you fewer scallops than your bull nose. I would personally use the toolpath with the most points and then mess with any smoothing settings on the cnc control to get the finish I want.

Thanks for your suggestion.. I didn't thought about the difference with a bull or ball.. I just assume a radius was a radius..

The feedrate was just to speed up the test itself.. I tried with half the feed and surface still didn't appear better, when it comes to those "steps" in the surface..

I tried to make it as one all the way around, but due to the top and bottom, but couldn't get it to work, probably due to the geometry of the blade, which is strangely curved in the bottom profile.. I have played with filters, but in Mastercam and on the machine as well.. It has several options, depending on what type of machining you do, but that didn't help either.. 

I have made some test since I posted this with the Unified tool-path, and it actually looks quite much better.. Not perfect still, but maybe with a ballmill I will archieve what I was hoping for..  

 

 

11 minutes ago, #Rekd™ said:

+1 to using a ball nose end mill.

 

Also you can try using "Angle Increment" in Tool Axis control to make the vectors closer together (using a small number like 0.5 degrees or smaller)

I have already played with this as well, tried everywhere from 0.1 to 1mm in Angle increment.. Generally the more smooth I program the toolpath the worst it looks on the machine..

 

[crazy^millman]

Are you using G61.1 or G61.2? Has the Table and Work Piece Coordinates issue been sorted out on your machine? What version of Smooth Control are you running. I uncovered a major flaw with Smooth controls last year when using G61.2 for 5 axis smoothing that was causing the machine to crash for Honda.

Mazak Kentucky has been telling CNC software they should be using Work Piece Coordinates for all the settings to run the machine when it should be Table Coordinates. I had what should have been the crown jewels of toolpath cutting the Indy Car Block for Honda on an Intergex and it was okay, but not there. After 10 months of run around from a lot of different places once we switched everything over to Table Coordinates and got al the parameter on the machine matching and in the MT Environment it was a night and day difference. I looked through all the releases notes for Smooth Controls for MT Machine and haven't seen mention of this change.

The next issue was the G61.2 R values for 5 Axis filtering not working correctly. The book kept saying use G61.1 for 5 axis filtering, but they were not working in G43.4 it was only when we found G61.2 that we started to see real improvements on the machine. R Mazak Japan got involved all the way up to Vice President of Mazak Japan. They had to make an software update for the machine to fix this issue. What is the age of the machine and what version of software is it running? Has this issue be resolved on this machine? Reach out to Craig Finney an Applications Engineer on the West Coast he should remember everything I went through with Honda on their machine.

[JFGuffie]

5 minutes ago, crazy^millman said:

Are you using G61.1 or G61.2? Has the Table and Work Piece Coordinates issue been sorted out on your machine? What version of Smooth Control are you running. I uncovered a major flaw with Smooth controls last year when using G61.2 for 5 axis smoothing that was causing the machine to crash for Honda.

Mazak Kentucky has been telling CNC software they should be using Work Piece Coordinates for all the settings to run the machine when it should be Table Coordinates. I had what should have been the crown jewels of toolpath cutting the Indy Car Block for Honda on an Intergex and it was okay, but not there. After 10 months of run around from a lot of different places once we switched everything over to Table Coordinates and got al the parameter on the machine matching and in the MT Environment it was a night and day difference. I looked through al the releases notes for Smooth Controls and haven't seen mention of this change.

The next issue was the G61.2 R values for 5 Axis filtering not working correctly. The book kept saying use G61.1 for 5 axis filtering, but they were not working in G43.4 it was only when we found G61.2 that we started to see real improvements on the machine. R Mazak Japan got involved all the way up to Vice President of Mazak Japan. They had to make an software update for the machine to fix this issue. What is the age of the machine and what version of software is it running? Has this issue be resolved on this machine? Reach out to Craig Finney an Applications Engineer on the West Coast he should remember everything I went through with Honda on their machine.

Thanks for your input.. 

 

The machine has just passed one year of age by now and is a Smooth AI.. I'm running with G61.1 followed by a P6.. I have tried to change to P7, which should make more smooth surface.. It also runs more slowly, but it just increases the steps everytime it slows down..  

Below here in an example from the output.. Maybe that will help to explain something.. :)

N3 (OPERATION 3)
(Ø16 R2 BULLMILL LONG)
G0 G90 G18 G40 G49 G80
G69
G10.9 X0
M200 (1ST SPINDLE MILL MODE)
G17 G54
T#501 M6 T#502
M821 (ACCURACY LEVEL)
G61.1 P6
M108 (UNCLAMP B)
G90 G0 G53 B95.1
#150=#3020
#151=#[60000+#150]
#152=#151+170.2
#153=-46.275-[#152-#152*COS[95.1]]
G0 G43 Z#153
M212 (UNCLAMP C)
C194.125
M8
G97 S12000 M3
G94
G43.4 X139.269 Y-7.763 Z-46.275 C194.125 B95.1
X66.558 Y-7.763 Z-39.785 C194.125 B95.1
G5P2 (HIGH SPEED ON) 

 

I'll contact my local Mazak guy and ask him acc. to what you write.. Maybe he can check up on something, since I have no experience with G61.2 and how to use it..

 

[crazy^millman]

5 minutes ago, JFGuffie said:

Thanks for your input.. 

 

The machine has just passed one year of age by now and is a Smooth AI.. I'm running with G61.1 followed by a P6.. I have tried to change to P7, which should make more smooth surface.. It also runs more slowly, but it just increases the steps everytime it slows down..  

Below here in an example from the output.. Maybe that will help to explain something..

N3 (OPERATION 3)
(Ø16 R2 BULLMILL LONG)
G0 G90 G18 G40 G49 G80
G69
G10.9 X0
M200 (1ST SPINDLE MILL MODE)
G17 G54
T#501 M6 T#502
M821 (ACCURACY LEVEL)
G61.1 P6
M108 (UNCLAMP
G90 G0 G53 B95.1
#150=#3020
#151=#[60000+#150]
#152=#151+170.2
#153=-46.275-[#152-#152*COS[95.1]]
G0 G43 Z#153
M212 (UNCLAMP C)
C194.125
M8
G97 S12000 M3
G94
G43.4 X139.269 Y-7.763 Z-46.275 C194.125 B95.1
X66.558 Y-7.763 Z-39.785 C194.125 B95.1
G5P2 (HIGH SPEED ON) 

 

I'll contact my local Mazak guy and ask him acc. to what you write.. Maybe he can check up on something, since I have no experience with G61.2 and how to use it..

 

Well we found using G61.1 and G43.4 with every setting wouldn't give good 5 Axis motion. It was not until we switched to G61.2 that we started getting swmooth 5 Axis motion on the machine. I also see it not being output in the correct place it should come after G43.4 not before.

Here is ho we ran it on their machine.

N10
(OPERATION # 48)
(FINISH RADIUS IN TOP CORNER #6A)
G91 G28 X0. Y0.
G28 Z0.
M108
G90 G0 B0.
M107
(T040  |  8. BALL ENDMILL  | DIA. -  8)
G10.9 X0
M901
M200
T040.02 T041 M6
G94
G97 S8000 M03
G58
G17
M108 M212
G0 B89.107 C66.247
M212
G43.4 H40 X-10.217 Y32.156 Z-222.147
M08
G94
G61.2
G05 P2
G94 G1 C66.247 B89.107 F2500.
X-50.243 Y-58.795 Z-223.695
X-56.284 Y-72.522 Z-223.929
X-58.298 Y-77.098 Z-224.007 F1250.
X-58.256 Y-77.128 Z-224.018
X-58.207 Y-77.166 Z-224.032
X-58.161 Y-77.207 Z-224.046

 

[crazy^millman]

The other thing is 300 micron is too loose a point setting for a part like that. i would also look for a oval form cutter and not use a ball or bull on this part. Use Unified with these setting on the tool axis control to really get the most use out of the tool. 

[crazy^millman]

Here is a file with toolpaths thrown on it using a Taper Form tool.

Dropbox link

[#Rekd™]

21 minutes ago, crazy^millman said:

using a Taper Form tool

Hi Ron,

What toolpaths can support the barrel/ taper form tools?

 

[crazy^millman]

6 minutes ago, #Rekd™ said:

Hi Ron,

What toolpaths can support the barrel/ taper form tools?

 

Unified is now the only I am aware of. Maybe someone from CNC Software can chime in.

[rgrin]

Multiaxis pocket I assume still supports them.

Heres a video from the Mastercam youtube page showing it. https://www.youtube.com/watch?v=T1YwR45pbLA

 

I know I saw another video there that showed them using a taper form cutter to finish a wall. Almost certain it also used Multi axis pocket

[Aaron Eberhard]

Yep, Unified and Pocket in Multiaxis, and all of the 3d high speed stuff (equal scallop/waterline/etc.). 

[JFGuffie]

On 8/30/2023 at 9:46 PM, crazy^millman said:

Here is a file with toolpaths thrown on it using a Taper Form tool.

Dropbox link

Sorry for not responding before, but was out of office end of last week.. 

 

Thanks for the help.. It has been very helpful.. I see that I still have a lot to learn..

 

[crazy^millman]

3 hours ago, JFGuffie said:

Sorry for not responding before, but was out of office end of last week.. 

 

Thanks for the help.. It has been very helpful.. I see that I still have a lot to learn..

 

I have been in this profession over 35 years and I am always learning something. When we think we have arrived in this profession trust me you will be knocked down a few notches real quick. Please keep asking questions and posting files to learn even more. That is what makes this forum work is people helping each other.