What feedrates, and depth of cut?
I'd lower the rpm, and take shallower cuts.
Hey G'day folks,
Some advice please..
I have a number of 9/11 mm perspex sheets varying sizes average sizes 12 x 14" thereabouts.
Thought I'd give a go at doing some reverse bas reliefs in the medium. I did this using a tapered ball nose 1mm radius. (I thought I'd try the tapered)
It was my first try conventional offset, started at the middle of the piece and ended up with a nice piece. Its come out good enough for me to use as a mold and try my hand at Cold Casting a couple extra. (something else on my bucket list to have a crack at)
Now I have tried unsuccessfully to do some other work, using single spiral end mill 2mm and 3mm, (cutting some pieces for other small projects that I have) with little to no success!
Spindle speed, 18000 according to doctor google but that didn't do me much good, the bit was not ejecting the shrapnel well enough, particularly doing a profile cut.
Faster spindle feeds, only melted the perspex which then stuck to the bit cooling and making problems. The melted bits got progressive larger and well you can imagine the result.
Tried slower feeds and speeds, ended up snapping a couple of bits.
Using a 6mm endmill produced somewhat better results but its too large for what i need it to do.
Trying to peck some holes for threading the bits tend to melt their way through rather than cut.
If anyone has worked with perspex, a tip on the type of bit to use, speed and feeds would be great.
At the moment it seems more an accident that I got a nice piece rather than by design.
Dr Google isn't helping much.
Cheers,
Steve
Similar Threads:
What feedrates, and depth of cut?
I'd lower the rpm, and take shallower cuts.
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Well the item I finished was done in a single pass, and it turned out fine with the tapered bit . 150mm/sec
The others cuts I did, at 1.5mm / 2mm / 3mm depth of cut 60 mm/sec. I don't know how much slower to go, without causing a problem with rubbing and creating more heat.
Problem I had in doing more passes and shallow depth was the chips were not coming out being hot they were adhering to the trench and change to a brittle property which the end mill was having problems working through.
rpm you think to high, ok can always go lower.. I can afford to loose a few more bits.
Cheers and ty for your reply.
Steve
Cutting slower is the opposite of what you want. If it's hot, or melting, you usually want either higher feedrates,or lower rpm, or both
It's hard to clear the chips when using small bits. What you really need is an air blast, or something else to help cool and get the chips out
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
I just finished reading an article suggesting the same thing.. go as fast as practicable to avoid heating..... ty for your reply
Steve
Try using a 50-50 mix of dish detergent and water as coolant. Just brush it on
Dave
In the words of the Toolman--If you didn't make it yourself, it's not really yours!
Remember- done beats perfect every time!!
I may give that a go, seeing as my wife has already objected to putting a couple of pieces in the freezer overnight.
Cheers,
Steve
Hi,
18,000rpm is very fast. I cut perspex at around 1,500 - 3,000 rpm with a 1/8" single flute cutter. I have a fog buster and use it to blow air with no coolant. The air helps to clear the chips and cool things down.
You need to adjust things to find the sweet spot. If you break bits, it could be that the feed rate is too fast. If you slow it down, then the plastic might melt, so you then need to take shallower cuts so the feed rate can be increased.
https://www.homanndesigns.com/index....roducts_id=131
Cheers,
Peter
-------------------------------------------------
Homann Designs - http://www.homanndesigns.com
Hey Peter G'day,
Thank you for that information, ok that's a big difference in spindle speed. I can see the merit in that, I will give that a try in the morning. When you say shallow cuts are we talking less than 1mm ? so far I have been taking about 1.5 mm but I can take less if need be.
I will start with your tips and see how I go from there.
Thank you for taking the time pitch in with a reply.
Cheers,
Steve
But what feedrate at 3000rpm? You should get similar results at 18,000 rpm with a 6x higher feedrate.
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
My expertise is more in electronics rather than machining. I think my cuts would be 1mm at most.
Also, it is my understanding that the depth of cut should be no greater than 30% of the cutter diameter.
It’s all about the chip loading on the cutter, then compromises for the material machine rigidity etc.
Peter
Well Im off to the workshop to try all this out, if 30% of cutter diam is meant to be depth of cut Im pretty safe there then. So I am either going too slow or not fast enough. Or the spindle speed is to quick or will be too slow.. Will have some results later in the afternoon.
Cheers and ty for pitching in.
Steve
Ok did some testing today, slow spindle speed works ok, 18k spindle speed and fast works ok as well in straight lines. Where its coming unstuck is with UCCNC not to much of a problem with Mach3.
Whats happening and I don't know how to fix this with UCCNC, If I make straight line cuts and set machine to say, 50mm sec not an issue. As soon as I do a curve or a zig zag in the cut UCCNC ignore the speed its set at goes slow ramps down and the heating problems with the cut.
eg if I do a square seems to be ok, if I do a square with rounded corners Im in trouble.
Mach3 not having an issue cutting round corners in the perspex, it slows slightly for the corner but pretty much full steam ahead. spend an hour or so trying to spot why and have given up for the night the workshop was getting chilly and my patience was worn.
If anyone has a clue what Im talking about assistance would be appreciated.
Cut depth I used all day was 1mm.
Cheers,
Steve
A cut depth of 1 mm is fine with a 6 mm ball end mill. With a 1 mm ball end mill it is ... perhaps a little optimistic?
Otherwise, 2,000 rpm, 100 mm/minute, with air blast turned ON! A water mist will help a lot.
Cheers
Roger
Hey Roger ty for the advice,
I'm not using a 1mm ball end sry if I've given that impression. Using a 3mm single flute. I agree a 1mm ball end would be optimistic!! LOL.
I think where my issue is using UCCNC atm. I seem to be doing fine with mach3 it is zipping along, where as UCCNC atm seems to have a mind of its own even though I have set it at 50/80mm sec I don't think its traveling faster than 20mm...
I'm sure there is an over ride somewhere.
Cheers mate,
Steve
In UCCNC, try increasing the error tolerance CV settings, for both the corner error and linear error.
Part of the reason that Mach3 is running faster is that it really has no path deviation control, so it's priority is to maintain velocity, regardless of accuracy.
UCCNC prioritizes accuracy, which can result in slower moves required to maintain the desired accuracy.
Higher acceleration settings can help a lot. Machines with low acceleration may run much slower than you'd like.
UCCNC also sometimes has issues with transitions to and from arcs (G2/G3), where it slows down at the transitions. Again, faster accel will reduce or minimize the issue. CNC Drive is supposed to start working on a new trajectory planner in the near future that will hopefully resolve this issue.
What does your g-code look like?
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Mike G'day,
Ty for the tips well appreciate and ty for posting.
Cheers,
Steve
Hey Gerry G'day,
Awesome ty for that information, that would explain a lot thats going on. As there is a big difference between the two software.
GCode please see attached file hrmmm ok dont know how to attach a file or least cant see how, pictures yes, links to video yes file no.. Ok Ill cut paste a portion of the file then hopefully will be enough for you to see whats what. If you want to see the whole file if you can give me a clue as to how to attach it in this forum.
cheers,
Steve
( profile cut )
( File created: Wednesday May 29 2019 - 09:51 AM)
( for Mach2/3 )
( Material Size)
( X= 305.000, Y= 320.000, Z= 10.000)
()
(Toolpaths used in this file
(Profile 2)
(Tools used in this file: )
(1 = End Mill {0.125 inch})
N100G00G21G17G90G40G49G80
N110G71G91.1
N120T1M06
N130 (End Mill {0.125 inch})
N140G00G43Z25.010H1
N150S12000M03
N160(Toolpath:- Profile 2)
N170()
N180G94
N190X0.000Y0.000F1270.0
N200G00X79.746Y42.747Z10.000
N210G00Z5.000
N220G1Z-1.833F508.0
N230G3X81.334Y41.160I1.587J0.000F1270.0
N240G1X83.921
N250G1X90.078
N260G1X90.431Y41.150
N270G1X90.755Y41.121
N280G1X91.075Y41.074
N290G1X91.390Y41.009
N300G1X91.700Y40.927
N310G1X92.005Y40.827
N320G1X92.304Y40.710
N330G1X92.598Y40.576
N340G1X92.886Y40.426
N350G1X93.168Y40.260
N360G1X93.444Y40.077
N370G1X93.712Y39.879
N380G1X93.972Y39.665
N390G1X94.225Y39.436
N400G1X94.468Y39.193
N410G1X94.702Y38.936
N420G1X94.926Y38.664
N430G1X95.140Y38.380
N440G1X95.342Y38.083
N450G1X95.533Y37.773
N460G1X95.712Y37.451
N470G1X95.878Y37.119
N480G1X96.030Y36.775
N490G1X96.169Y36.421
N500G1X96.293Y36.058
N510G1X96.403Y35.685
N520G1X96.496Y35.304
N530G1X96.574Y34.915
N540G1X96.636Y34.517
N550G1X96.680Y34.113
N560G1X96.708Y33.702
N570G1X96.717Y33.267
N580G1Y11.618
N590G3X98.305Y10.030I1.588J0.000
N600G1X109.507
N610G1X114.682
N620G1X124.451
N630G3X126.038Y11.618I0.000J1.588
N640G1Y33.356
N650G1X126.048Y33.786
N660G1X126.075Y34.192
N670G1X126.119Y34.591
N680G1X126.180Y34.983
N690G1X126.258Y35.368
N700G1X126.352Y35.744
N710G1X126.461Y36.112
N720G1X126.584Y36.471
N730G1X126.723Y36.821
N740G1X126.875Y37.160
In that code, the big "arc" is made up of multiple G1 moves, and slowed down quite a bit. By increasing the error tolerance settings to 0.1, it ran at a fairly steady feedrate. You may need to play with the settings a bit, as acceleration plays a role.
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)