HSMAdvisor vs G-Wizard vs Free calc?! - Page 3


Page 3 of 3 FirstFirst 123
Results 25 to 35 of 35

Thread: HSMAdvisor vs G-Wizard vs Free calc?!

  1. #25
    Registered
    Join Date
    Nov 2017
    Posts
    91
    Downloads
    0
    Uploads
    0

    Default Re: HSMAdvisor vs G-Wizard vs Free calc?!

    Thanks. I actually watched that recently. Very helpful.

    Like everything else, if a newbie followed same data like a pro, it won't have the same result! There are too many other variables at play and you can't fix all. I am convinced it will come with experience and experimentation.

    Today, the calculator showed me that I can indeed slot through a 1.2" 6061-T6 using 3800 RPM 8 IPM, with 0.5" 2F HSS, and using 0.6" DOC and of course 1/2" WOC as it's the Dia. This is using Tormach 770 as selected machine but dialed down. Didn't work.

    So instead as a learning operation, I did it in multi-pass with each pass different RPM and Feeds. DOC varied between 0.05" and 0.2". This is all good, it's all part of the learning curve and every newbie got to go through testing.


    Quote Originally Posted by C*H*U*D View Post
    Something like this?



    Attached Thumbnails Attached Thumbnails HSMAdvisor vs G-Wizard vs Free calc?!-a1-jpg   HSMAdvisor vs G-Wizard vs Free calc?!-a2-jpg  


  2. #26
    Registered zero_divide's Avatar
    Join Date
    Sep 2012
    Location
    Canada
    Posts
    247
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by narrobb View Post
    Thanks. I actually watched that recently. Very helpful.

    Like everything else, if a newbie followed same data like a pro, it won't have the same result! There are too many other variables at play and you can't fix all. I am convinced it will come with experience and experimentation.

    Today, the calculator showed me that I can indeed slot through a 1.2" 6061-T6 using 3800 RPM 8 IPM, with 0.5" 2F HSS, and using 0.6" DOC and of course 1/2" WOC as it's the Dia. This is using Tormach 770 as selected machine but dialed down. Didn't work.

    So instead as a learning operation, I did it in multi-pass with each pass different RPM and Feeds. DOC varied between 0.05" and 0.2". This is all good, it's all part of the learning curve and every newbie got to go through testing.
    It probably stalled the spindle.

    Power calculations only make sense when feedrate is close to ideal values.

    When you have to go so deep, HSMAdvisor would reduce your feedrate considerably which would lead to more friction and spindle stalling.

    http://hsmadvisor.com/
    Advanced Feed and Speed Calculator


  3. #27
    Registered
    Join Date
    May 2016
    Location
    United States
    Posts
    137
    Downloads
    0
    Uploads
    0

    Default Re: HSMAdvisor vs G-Wizard vs Free calc?!

    1/2" is on the larger side for these machines. If you are trying stuff out, try a smaller endmill. Going with a smaller endmill then the slot needs to be will also give you a nicer finish on both walls.



  4. #28
    Registered
    Join Date
    Apr 2016
    Posts
    74
    Downloads
    0
    Uploads
    0

    Default Re: HSMAdvisor vs G-Wizard vs Free calc?!

    When I run the numbers on your slotting operation with a 1/2" end mill (that's a big frickin end mill for a 770 especially for a slotting op) I get this cutting data:

    Material: 6061-T6 Series Aluminum 95 HB
    Tool: 0.500in 2FL HSS None Solid End Mill
    Speed: 480.0 SFM/ 3668.8RPM
    Feed: 0.0032 in/tooth 0.0064 in/rev 23.48 in/min
    Chip Thickness: 0.0032 in
    Reference Chip load: 0.0032 in
    Engagement: DOC=0.17 in WOC=0.50 in
    Effective Dia: 0.500 in
    Cross Section: 0.33 x Dia.
    Power: 0.6HP
    MRR: 1.96 in³
    Torque: 0.84 ft-lb
    Max Torque: 5.73 ft-lb
    Cutting Force: 40.4 lb
    Deflection: 0.0022 in
    Max Deflection: 0.00500 in

    And even with my derated numbers for the machine I'd still work into this carefully with the feed slider. And plenty of coolant. If I was trying this with my fogbuster I'd have it aimed carefully and be looking for good chips instantly, or stop. Welding a ton of chips to a nice YG-1 1/2" isn't a good time.

    According to the calc there's no way no how for the 770 to take a full .6 DOC in 6061. It's miles short on HP. Low belt mode didn't make much difference. It's showing .17 for a realistic depth. It's just going to take several passes. And after that first pass the deeper you go the more difficult the chip evacuation and cooling will become. Maybe start with this for the first pass or two and then use less DOC for the remaining passes.

    OR you could whip up an adaptive clearing tool path and work through the slot. This cut with a 5/16 end mill has almost the same MRR (material removal rate) it would be just as fast, but will take a little more time because of the brief moves to start the next pass as it walks through. It would go at the full DOC though:

    Material: 6061-T6 Series Aluminum 95 HB
    Tool: 0.312in 2FL HSS None Solid End Mill
    Speed: 600.0 SFM/ 7337.6RPM
    Feed: 0.0032 in/tooth 0.0065 in/rev 47.69 in/min
    Chip Thickness: 0.0032 in
    Reference Chip load: 0.0032 in
    Engagement: DOC=0.60 in WOC=0.07 in
    Effective Dia: 0.312 in
    Cross Section: 0.42 x Dia.
    Power: 0.6HP
    MRR: 1.94 in³
    Torque: 0.42 ft-lb
    Max Torque: 1.40 ft-lb
    Cutting Force: 32.1 lb
    Deflection: 0.0013 in
    Max Deflection: 0.00400 in

    This has a much better chance of working though. Infinitely better chip evacuation, much lower torque, much longer tool life. I whipped up both in Fusion 360 for fun, about 2:36 to adaptive clear a 6" slot at .6" depth. The full slotting op with multiple depth passes was only a little faster at 2:13.

    This NYC CNC video from 2016 shows the basics of how to set up a tool path like this:
    https://www.youtube.com/watch?v=hGVf2GPqcv8

    This is good practice for me. If my numbers are screwed up bad, someone here will be sure to set me straight.



  5. #29
    Registered
    Join Date
    Nov 2017
    Posts
    91
    Downloads
    0
    Uploads
    0

    Default Re: HSMAdvisor vs G-Wizard vs Free calc?!

    Only just starting to learn these calculators, so maybe I am using it wrong? Here is my screen shot. I derated the Machine itself to 1.1 ft-lb Max torque and 0.8HP.

    I input the 0.6 DOC and then used the slider to adjust so all in the green, If I recall, I think it suggested 27 in/min then I put it down further. So does this mean even if all in the green, and the correct machine selected, the cut still can't be done?

    0.2" DOC using same data did cut (but the cutting noise made me think its right at the top of the torque/load), while 0.1" DOC was much smoother and easy on the ears! I still have miles to cover, but perfectly happy with going for the 770 and not the 440 as was initially planned.

    Thanks

    Attached Thumbnails Attached Thumbnails HSMAdvisor vs G-Wizard vs Free calc?!-cut-jpg  


  6. #30
    Registered
    Join Date
    May 2016
    Location
    United States
    Posts
    137
    Downloads
    0
    Uploads
    0

    Default Re: HSMAdvisor vs G-Wizard vs Free calc?!

    My 1100 wouldnt like a.6" DOC with a 1/2" endmill either.

    The calculators can get you close, but not always, and you will always find things that may work on paper but not in real life. That cut will chatter badly. You also have to consider flute length, you need them to be above the cut so the chips can evacuate.

    As time goes on you will figure out what the machine likes and doesnt.

    Again, try it with a 1/4" endmill To get a good surface finish, you want to have a tool smaller than the slot you are making.



  7. #31
    Registered
    Join Date
    Nov 2017
    Posts
    91
    Downloads
    0
    Uploads
    0

    Default Re: HSMAdvisor vs G-Wizard vs Free calc?!

    Quote Originally Posted by joshetect View Post
    Again, try it with a 1/4" endmill To get a good surface finish, you want to have a tool smaller than the slot you are making.
    Thanks. Yes, if it was for an actual item, i will go that route, but as I am just making mess and learning I thought of experimenting with used endmils, i got over 80 such 1/2" endmils with half-life or so.



  8. #32
    Registered
    Join Date
    May 2016
    Location
    United States
    Posts
    137
    Downloads
    0
    Uploads
    0

    Default Re: HSMAdvisor vs G-Wizard vs Free calc?!

    Thats another thing to consider then, as the tool wears, it requires more from the machine to make the cut.



  9. #33
    Gold Member mountaindew's Avatar
    Join Date
    Nov 2007
    Location
    earth
    Posts
    1591
    Downloads
    0
    Uploads
    0

    Default Re: HSMAdvisor vs G-Wizard vs Free calc?!

    Quote Originally Posted by narrobb View Post
    Thanks. Yes, if it was for an actual item, i will go that route, but as I am just making mess and learning I thought of experimenting with used endmils, i got over 80 such 1/2" endmils with half-life or so.

    Just my opinion, want good consistent results, use good quality cutters. Try one of those cutters shown in your pictures then throw something like a 3/8 yg alum max cutter that Tormach sells and see the difference while it quietly plows thru aluminum while you talk on the phone.

    I have some unknown cutters and even a few new ones in an old grizzly tool cutter set lol. Don't know exactly what they are good for as they do not cut anything well even wood . They do come in handy as alignment pins now and then.



  10. #34
    Registered
    Join Date
    Nov 2017
    Posts
    91
    Downloads
    0
    Uploads
    0

    Default Re: HSMAdvisor vs G-Wizard vs Free calc?!

    Agree about the cutters, hence my comment that even if newbie try the same feed/speed shown in various videos, milage may vary. As cutters brand/type/coating are variables.

    However, those 100's of cutters I got in the auction (if thats what you are referring to in pictures) are almost 95% OSG, fully traceable, with manufacturer details online including speed/feed. For example, this one attached 59181 OSG cost $106. The other one is over $90 as well. And still sharp enough that if rotated between two fingers with almost no pressure it will shave some skin. I actually did not mention OSG or part numbers when i offered them up, and one person who received their 40 end-mils box replied back pointing to me how costly these bits are when new.

    Quote Originally Posted by mountaindew View Post
    Just my opinion, want good consistent results, use good quality cutters. Try one of those cutters shown in your pictures then throw something like a 3/8 yg alum max cutter that Tormach sells and see the difference while it quietly plows thru aluminum while you talk on the phone.

    I have some unknown cutters and even a few new ones in an old grizzly tool cutter set lol. Don't know exactly what they are good for as they do not cut anything well even wood . They do come in handy as alignment pins now and then.


    Attached Thumbnails Attached Thumbnails HSMAdvisor vs G-Wizard vs Free calc?!-e1-png   HSMAdvisor vs G-Wizard vs Free calc?!-e2-png   HSMAdvisor vs G-Wizard vs Free calc?!-screen-shot-2018-01-24-11-22-a  


  11. #35
    Gold Member mountaindew's Avatar
    Join Date
    Nov 2007
    Location
    earth
    Posts
    1591
    Downloads
    0
    Uploads
    0

    Default Re: HSMAdvisor vs G-Wizard vs Free calc?!

    Quote Originally Posted by narrobb View Post
    Agree about the cutters, hence my comment that even if newbie try the same feed/speed shown in various videos, milage may vary. As cutters brand/type/coating are variables.

    However, those 100's of cutters I got in the auction (if thats what you are referring to in pictures) are almost 95% OSG, fully traceable, with manufacturer details online including speed/feed. For example, this one attached 59181 OSG cost $106. The other one is over $90 as well. And still sharp enough that if rotated between two fingers with almost no pressure it will shave some skin. I actually did not mention OSG or part numbers when i offered them up, and one person who received their 40 end-mils box replied back pointing to me how costly these bits are when new.


    I take that back
    I have some 1/4" carbide up-cut and compression cut router bits from osg they are 10 years old and still put a clear finish on Acrylic.
    I wont even admit what I paid for those at trade show prices even.



Page 3 of 3 FirstFirst 123

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

HSMAdvisor vs G-Wizard vs Free calc?!

HSMAdvisor vs G-Wizard vs Free calc?!