CAMheads CNC Router Forum By: CAMaster CNC

Go Back   CAMheads CNC Router Forum By: CAMaster CNC > The Water Cooler > The Water Cooler

Reply
 
Thread Tools Display Modes
  #11  
Old 10-19-2018, 08:37 PM
The real JP The real JP is offline
CAMaster Owner
 
Join Date: Mar 2017
Location: Oklahoma
Posts: 344
Default

Noooo don't tweak the post..

Those numbers are what you put in the tool speeds in Mozaik or Vectric. Just input higher feed speeds.

My smaller weaker stinger can run about 400ipm if everything is right.

Your bigger machine with a better vac should be able to do better. There is something in part size and corner speeds though.

I have not messed with my acceleration settings or anything like that, but I know it is a possibility.
__________________
Jpscustomshop@gmail.com

Industrial electrician by day, Cabinet and furniture maker by evening and weekend. Cnc newb.

June 2017 Stinger 3 SR48
3kw spindle, FTC, Laser, Recoil, Hurricane
V Carve, Mozaik
Reply With Quote
  #12  
Old 10-19-2018, 08:52 PM
The real JP The real JP is offline
CAMaster Owner
 
Join Date: Mar 2017
Location: Oklahoma
Posts: 344
Default

N70 S8000 [SET SPINDLE SPEED RPM] This means spindle rpm is set at 8000 in your software. it's fine

N75 M3 [SPINDLE ON]
N80
N85 G53 Z0 [LIFT Z TO TOP]
N90

N95 F150.0 XY [SET FEEDRATE FOR X AND Y] This means you have the speed set at 150 in your software. set 600 or machine max.

N100 F60.0 Z [SET FEEDRATE FOR Z] This means plunge rate at 60. set over 100

All this other stuff is basically goto this spot. line by line. It's like me telling you where to walk by telling you exactly where to place your foot and how far to pick it up. One step at a time.
Look through your win cnc booklet.

N175 G00Z2.218
N180 G00X37.877Y26.673Z2.218
N185 G00Z1.218
N190 Z-0.020
N195 G00Z2.218
N200 G00X34.190Y26.673Z2.218
N205 G00Z1.218
N210 Z-0.020
N215 G00Z2.218
N220 G00X34.190Y40.674Z2.218
N225 G00Z1.218
__________________
Jpscustomshop@gmail.com

Industrial electrician by day, Cabinet and furniture maker by evening and weekend. Cnc newb.

June 2017 Stinger 3 SR48
3kw spindle, FTC, Laser, Recoil, Hurricane
V Carve, Mozaik
Reply With Quote
  #13  
Old 10-19-2018, 10:40 PM
Doug S Doug S is offline
CAMaster Owner
 
Join Date: Jan 2018
Posts: 102
Default

A little more testing but strange issue:
After the results posted from the test files showing the estimated cut times, I went to my sheets and recorded the actual times to perform the same nest. The results were almost double in every case. see examples.

Sheet 1 estimated time: 3:83 actual: 5:42
Sheet 2 estimated time: 3:65 actual: 5:15
Sheet 3 estimated time: 6:63 actual: 11:36

So, what would cause this as it is showing all my parameters and such but not cutting as fast as it thinks it is.

Tomorrow I have two identical projects and I will run the first one as currently configured. For the second one, I will reset the speeds and change to the 1/2" dado bit and see what results we have.

Thanks again for all the assistance.
__________________
2014 Cobra 5x10 ATC w/ 10 hp spindle, Mozaik, 25 hp Becker High Vacuum Pump, 5 HP Oneida DC-Central Texas
Reply With Quote
  #14  
Old 10-19-2018, 10:55 PM
The real JP The real JP is offline
CAMaster Owner
 
Join Date: Mar 2017
Location: Oklahoma
Posts: 344
Default

Slowing down for corners and small parts that never get it out of slow mode.

I have not messed with it on my machine but you can change the acceleration and other settings in win cnc. Call Camaster tech or Maybe message Gary Campbell about it.

I know other guys know how to do this, but I don't know their names.

I wouldn't be too sad about those times though.
__________________
Jpscustomshop@gmail.com

Industrial electrician by day, Cabinet and furniture maker by evening and weekend. Cnc newb.

June 2017 Stinger 3 SR48
3kw spindle, FTC, Laser, Recoil, Hurricane
V Carve, Mozaik

Last edited by The real JP; 10-19-2018 at 10:57 PM.
Reply With Quote
  #15  
Old 10-20-2018, 08:33 AM
Gary Campbell's Avatar
Gary Campbell Gary Campbell is offline
CNC Tech & Trainer
 
Join Date: Dec 2012
Location: Marquette, MI USA
Posts: 2,762
Default

Sheet 1 estimated time: 3:83 actual: 5:42
Sheet 2 estimated time: 3:65 actual: 5:15
Sheet 3 estimated time: 6:63 actual: 11:36

Which CAM program are you using?
Have you made adjustments in that program to accommodate your machine, its acceleration, how you toolpath and the type of parts you are cutting?
__________________
Gary Campbell
CNC Technology and Training
The Ultimate Woodworking Machine
GCnC411@gmail.com
https://www.youtube.com/user/Islaww1/videos

"There are 10 kinds of people in the world. Those that understand binary logic, and those who don't"
Reply With Quote
  #16  
Old 10-20-2018, 11:33 AM
Doug S Doug S is offline
CAMaster Owner
 
Join Date: Jan 2018
Posts: 102
Default

Morning Gary,
Running Mozaik with WINCNC.

Have not gotten in to the speeds except where the specific bits call out a speed. It does not cover acceleration or traverse speeds that I am aware of.
__________________
2014 Cobra 5x10 ATC w/ 10 hp spindle, Mozaik, 25 hp Becker High Vacuum Pump, 5 HP Oneida DC-Central Texas
Reply With Quote
  #17  
Old 10-20-2018, 12:36 PM
Gary Campbell's Avatar
Gary Campbell Gary Campbell is offline
CNC Tech & Trainer
 
Join Date: Dec 2012
Location: Marquette, MI USA
Posts: 2,762
Default

The acceleration and rapid traverse are set by the factory and you shouldn't have to mess with them
__________________
Gary Campbell
CNC Technology and Training
The Ultimate Woodworking Machine
GCnC411@gmail.com
https://www.youtube.com/user/Islaww1/videos

"There are 10 kinds of people in the world. Those that understand binary logic, and those who don't"
Reply With Quote
  #18  
Old 10-21-2018, 03:21 PM
Doug S Doug S is offline
CAMaster Owner
 
Join Date: Jan 2018
Posts: 102
Default

Update on progress:

First let me state that I am a pure novice with this CNC thing. Never used one before and learning everyday. Additionally, I purchased this machine used and set it up and got it running without professional help except the fine folks here. So with all that said, I was not aware the values that came in Mozaik were simply suggestions. I have been using their factory setting for all tooling until yesterday, and after this topic.

Here are some of the changes I made:

Tool 1- 3/8" compression for cutout only went from 400 to 600 IPM.
Tool 2- 1/4" downshear for small dados went from 400 to 800 IPM
Tool 3- 3mm drill for assembly holes went from 400 to 1000 IPM
Tool 4- 5mm drill for shelf pins went from 400 to 1000 IPM
Tool 5- Dovetail bit-left at factory settings
Tool 6- 1/4" compression bit for cutting thin backs 400 to 600 IPM
Tool 7- 7mm drill for drawer hangers went from 400 to 1000 IPM
Tool 8- 8 mm drill for drawer guides in backs went from 400 to 1000 IPM
Tool 9- 1/2" downshear for 3/4" dados went from 400 to 800 IPM

The big changes were the 1/2" downshear for the dados-huge decrease in time. 2 passes instead of 5 and no tailings left behind.
Also changed the onion skins to RETURN SKIN so it cuts all the small parts first then comes back and cuts the onion skin before going to the large parts. This keeps the bigger pieces from pushing the small stuff. Works perfect.
Also sped up the plunge on all drilling from 60 to 150 and still getting perfect holes.

Thanks to everyone for their input. If anyone see anything stupid or crazy, drop it in here and lets discuss it.
I will keep looking for ways to trim more time, one being getting my offload table in full operation. Heck, half the time is in sorting and getting the table ready.
Have a great day.

Doug S
__________________
2014 Cobra 5x10 ATC w/ 10 hp spindle, Mozaik, 25 hp Becker High Vacuum Pump, 5 HP Oneida DC-Central Texas

Last edited by Doug S; 10-21-2018 at 06:41 PM.
Reply With Quote
  #19  
Old 10-21-2018, 04:59 PM
The real JP The real JP is offline
CAMaster Owner
 
Join Date: Mar 2017
Location: Oklahoma
Posts: 344
Default

I think those speeds seem like they would be nice to get. Your machine is mucho more grande than mine.

There are feeds and speeds apps for your phone. I have the us router tools one.
I think the biggest deal is experience.
You want a good cut quality and a good speed. You don't want to spin fast prm and slow feeds, burn your bit like that.

You also can't feed faster than it can do a good job cutting, might break a smaller bit or just make an ugly cut that you have to redo.

Nothing is easy or obvious when a person is new. I know that feeling well.

Just straight line cut some material at say 18000rpm and try different feed speeds. See where it is that you get a cut you like and that is your speed for that bit. Kind of simple, but it works.

Also, something I just learned in Mozaik cnc in the cnc tooling / cutout options you can have everything but the final through cut be slightly offset. So the final cut you make only removes .015 or so and hopefully leaves a really nice edge.
Attached Images
File Type: jpg Capture.jpg (17.2 KB, 12 views)
__________________
Jpscustomshop@gmail.com

Industrial electrician by day, Cabinet and furniture maker by evening and weekend. Cnc newb.

June 2017 Stinger 3 SR48
3kw spindle, FTC, Laser, Recoil, Hurricane
V Carve, Mozaik
Reply With Quote
  #20  
Old 10-21-2018, 06:17 PM
Doug S Doug S is offline
CAMaster Owner
 
Join Date: Jan 2018
Posts: 102
Default

My machine is rated at 1800 rapid but I feel much more speed could be pushing the holddown.
I was amazed at the holddown when the items cut in the proper order. I have been a little dissapointed in my pump recently as it would let loose on small parts but is was due to them being cut all the way first and then being pushed by the next piece.
That appears to be gone with the new RETURN SKIN method.works like a champ.

Thanks again for all the knowledge. I will continue to play with the height above the material to keep the drill stroke down.
__________________
2014 Cobra 5x10 ATC w/ 10 hp spindle, Mozaik, 25 hp Becker High Vacuum Pump, 5 HP Oneida DC-Central Texas
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 On

Forum Jump


All times are GMT -4. The time now is 04:38 AM.


Powered by vBulletin® Version 3.8.4
Copyright ©2000 - 2018, Jelsoft Enterprises Ltd.