CAMheads CNC Router Forum By: CAMaster CNC

Go Back   CAMheads CNC Router Forum By: CAMaster CNC > Tips & Techniques > General Discussion

Reply
 
Thread Tools Display Modes
  #1  
Old 06-18-2017, 08:28 PM
fcfoley fcfoley is offline
CAMaster Owner
 
Join Date: Mar 2015
Location: Newan, Georgia
Posts: 57
Default Machining Times

Today I made a 24" Aztec Calendar. The detail is amazing. I'm still amazed at what can be made with my machine. This leads me to my question. What variables can impact overall machining time. On this particular project I set all parameters to max. XY speed at 500ipm Z at 300ipm and Z clearance at .22. The project was cut with a 1/2 90deg v-bit. Total machine time was 4 hours 15 minutes. I understand the design makes it impossible to attain any of those speed parameters. I got the design from Peter at CNCNutz. I asked him how long it took for him to machine and he said just under 3 hours at 100ipm. I am confused with why it took longer. I would understand if Peter was running a Cobra or some other similar machine but he's not. So what am I missing?

__________________
Frank
Stinger II (SR-44)
3.0 kW Spindle w/speed control
Index Lathe
Performance kit, VCarve Pro 8.0
Reply With Quote
  #2  
Old 06-18-2017, 09:23 PM
Gary Campbell's Avatar
Gary Campbell Gary Campbell is offline
CNC Tech & Trainer
 
Join Date: Dec 2012
Location: Marquette, MI USA
Posts: 2,237
Default

Frank...
Asked and answered...
" I understand the design makes it impossible to attain any of those speed parameters." So why would you do that?

You set feeds higher than the machine could achieve. Therefore it was fighting itself trying to achieve those speeds. You need to set the feedrates to what would make the machine "happy". Find out how fast the Z can run that type of file and match that with the X and Y. That is your fastest cut.

My guess is, and you can try this aircut, set the feedrates at 150 in the XY and Z and get a faster cut time. If you wish to know why, restart your file with the spindle, dust and vacuum if you used it, all off so that you can hear the MACHINE. Then run the file at the feedrates I gave you and hear how different it sounds.

I also suggest that if you are looking to minimize machining times that you set your safe Z to .1

This is the bicycle vs. Corvette in a gymnasium race analogy, except that there is a maze drawn out in the gym, making it easier for the bicycle to win.
__________________
Gary Campbell
CNC Technology and Training
GCnC411@gmail.com
https://www.youtube.com/user/Islaww1/videos
www.cncseminars.com

"There are 10 kinds of people in the world. Those that understand binary logic, and those who don't"

Last edited by Gary Campbell; 06-18-2017 at 11:38 PM.
Reply With Quote
  #3  
Old 06-19-2017, 08:12 PM
fcfoley fcfoley is offline
CAMaster Owner
 
Join Date: Mar 2015
Location: Newan, Georgia
Posts: 57
Default

*UPDATE*
Gary I somewhat understand the point your making. So today for nearly 12 hours I ran multiple configurations of XY and Z speeds and doing test of 50 minutes long and determining any improvement by the number of lines of code completed in that time. It appeared the best setting was XY 100ipm Z60ipm. Additionally I reduced the Z clearance from .22 to .1. The end result was the program went from 255 minutes to 241 minutes, a savings of 14 minutes. I am attributing the bulk of that time savings to reducing the Z clearance.

While this is an improvement I still don't understand how one individual can run this in under 3 hours and it is taking me 4 hours.

One last think, if you were running this on a Cobra would it be under the same constraints that the XY speeds can not be obtained due to the amount of Z operations?

Thanks again for your help.
__________________
Frank
Stinger II (SR-44)
3.0 kW Spindle w/speed control
Index Lathe
Performance kit, VCarve Pro 8.0
Reply With Quote
  #4  
Old 06-19-2017, 10:51 PM
Charlie_L Charlie_L is online now
Stinger II Owner
 
Join Date: Mar 2012
Location: La Crosse, Wisconsin
Posts: 1,233
Default

Frank,
I'm curious, did you increase the z speed to equal the x and y too? You will notice a difference I suspect when you do that. Yes, the 0.1 clearance helps a lot too.
__________________
Charlie L
Stinger II, 48 by 48, 1.7 kW Spindle, FTC + Laser + Recoil + Vacuum, July 2012
WinCNC 2.5.03, Aspire 4, PhotoVCarve, Windows 7 Pro SP1
Reply With Quote
  #5  
Old 06-20-2017, 12:02 AM
Bruce Page Bruce Page is offline
Stinger I Owner
 
Join Date: Dec 2012
Location: Albuquerque, NM
Posts: 1,349
Default

I don’t think your time is out of line. I did a 15” Aztec and it took ~ 4 hrs IIRC.
My feed was 100ipm x 100ipm x 80ipm on Z, .1 safe Z
There are a ton of nodes in that model.
Attached Images
File Type: jpg Aztec Calendar 1a.jpg (80.9 KB, 45 views)
__________________
Bruce Page
Retired Hobbyist
Stinger 1 SR23
FTC
Laser Pointer
HSD 1.7kw Spindle
KRS USB Keypad
Mick Martin Table
Aspire 8.5, WinCNC
Chips-a-flyin’
brucep128@gmail.com
Reply With Quote
  #6  
Old 06-20-2017, 08:00 AM
Gary Campbell's Avatar
Gary Campbell Gary Campbell is offline
CNC Tech & Trainer
 
Join Date: Dec 2012
Location: Marquette, MI USA
Posts: 2,237
Default

Frank...
Were any of your speed configurations done with the X, Y and Z speeds set equal? That is what you want. Equal speeds and as fast as the Z can go without clunking.

It is better to cut "x" amount of lines out of a file and then time it for comparison than to apply your logic to how many lines run. The lines are not equal time.

In this type of file speeds are being limited by the length and angle of vector. Of course a more powerful machine will cut them faster, but not as great a difference as you might think.
__________________
Gary Campbell
CNC Technology and Training
GCnC411@gmail.com
https://www.youtube.com/user/Islaww1/videos
www.cncseminars.com

"There are 10 kinds of people in the world. Those that understand binary logic, and those who don't"
Reply With Quote
  #7  
Old 06-20-2017, 02:25 PM
drummerjg drummerjg is offline
CAMaster Owner
 
Join Date: Dec 2016
Location: Addison, PA
Posts: 171
Question

Just for grins, I went out to the CncNutz site and downloaded the Aztec calendar file. When I loaded it into Aspire and did a run time estimate it came back and told me 3hr 15min, plus 4min to cut the profile. That was using the tool paths associated with the file. So I guess Im curious why Franks run time is so much longer. My experience ( and it is VERY limited, mind you) has been the estimated cut times from Aspire are usually longer than the actual machine time.
Im guessing my Stinger would take about 3 hours to make the calendar. Would there be any run time differences between Aspire & V Carve???
__________________
Joe Garber
Retired Hobbyist
Stinger 1 SR24
FTC
Laser Pointer
HSD 1.7kw Spindle
Indexing Lathe
WinCNC
Aspire 9
trommlerjg@gmail.com


How to count to 10 in software:
1,2,3,95,NT,2000,XP,Vista,7,8,10
Reply With Quote
  #8  
Old 06-20-2017, 05:49 PM
Gary Campbell's Avatar
Gary Campbell Gary Campbell is offline
CNC Tech & Trainer
 
Join Date: Dec 2012
Location: Marquette, MI USA
Posts: 2,237
Default

The Machining time estimate in any software is just that. An estimate. They can be off by half or double until you get the scale factor set for your machine, its speeds and acceleration, the way you as an individual toolpath and the vector type.

If you wish to know how long it will take to cut, aircut the file. Best "estimate" there is.
__________________
Gary Campbell
CNC Technology and Training
GCnC411@gmail.com
https://www.youtube.com/user/Islaww1/videos
www.cncseminars.com

"There are 10 kinds of people in the world. Those that understand binary logic, and those who don't"
Reply With Quote
  #9  
Old 06-20-2017, 08:26 PM
fcfoley fcfoley is offline
CAMaster Owner
 
Join Date: Mar 2015
Location: Newan, Georgia
Posts: 57
Default

Today I ran my last and final test. I was surprised with the results and came away with a different prospective when it comes to setting feed rates.

I first want to say that every job is different and depending on complexity of the job will greatly affect machining times. Additionally, cutting out panels where X and Y speed can be utilized to their fullest these test results would not apply.

Here's what I did. I ran the Aztec file from the same start point and noted the time it took to reach 30,000 lines and 50,000 lines as tracked on WINCNC. I ran all test with a .1 Z clearance. Below are the results.

XY 300IPM, Z 300IPM
30,000 = 36:28
50,000 = 59:36

XY 150IPM, Z 150IPM
30,000 = 36:28
50,000 = 59:35

XY 100IPM, Z 100IPM
30,000 = 36:22
50,000 = 59:27

XY 50IPM, Z 50IPM
30,000 = 36:56
50,000 = 60:37

Surprisingly (at least to me) was the fastest operation (at least for this file) was the 100IPM. Furthermore, the difference between the 300IPM and 50IPM was just 1 minute after an hour of operation.

I am guessing that similar results would be obtained if the project did not have a large surface area that would take advantage of faster XY speeds and there was a significant amount of Z operations.

For me this changes my thought process when I am determining feed rate. Of course any feed rate adjustments would also effect router/spindle speed.

If I am missing something in this test or it is flawed please let me know.

Thanks
__________________
Frank
Stinger II (SR-44)
3.0 kW Spindle w/speed control
Index Lathe
Performance kit, VCarve Pro 8.0
Reply With Quote
  #10  
Old 06-20-2017, 10:00 PM
Gary Campbell's Avatar
Gary Campbell Gary Campbell is offline
CNC Tech & Trainer
 
Join Date: Dec 2012
Location: Marquette, MI USA
Posts: 2,237
Default

Frank...
First and foremost, thank you for taking the time to do this and report your results. Lets take it a bit further and it may make sense.

By your results you can see that (1st example) the machine executed 30,000 lines of code in 36:28 or 2188 seconds, or 13.7 lines per second. Remembering that in each line of code the machine has to either accel and decal or maintain speed, depending on your settings.

Those setting are feedrate acceleration (especially in the Z), autoarcfeed, smoothing and the axisvel "c" setting. If you do this type of file often you may be able to shave more time off than you think. Bad news is that other types of files will not be optimized.

Now you know why I recommend 100ipm XYZ for VCarve and 3D files for most machines in my feeds and speeds classes. There is less to gain from the larger machines with this type of file than most would believe. It takes special settings and LOTS of reduction and torque to maintain speed while moving 3 axes and going around corners.

There are a few examples throughout, but the most obvious is at 4:28 into this video: https://www.youtube.com/watch?v=FdyZLi6phVI

Watch the cornering speed
__________________
Gary Campbell
CNC Technology and Training
GCnC411@gmail.com
https://www.youtube.com/user/Islaww1/videos
www.cncseminars.com

"There are 10 kinds of people in the world. Those that understand binary logic, and those who don't"
Reply With Quote
Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off

Forum Jump


All times are GMT -4. The time now is 07:31 AM.


Powered by vBulletin® Version 3.8.4
Copyright ©2000 - 2017, Jelsoft Enterprises Ltd.