Author Topic: Going over to the dark (CNC) side!  (Read 10387 times)

Offline Muzzer

  • Full Member
  • ****
  • Posts: 22
Re: Going over to the dark (CNC) side!
« Reply #60 on: March 09, 2019, 01:02:02 PM »

Murray,

Good to see you chipping in here, would definitely be interested in how long this would take you as having seen your machine in action it can shift metal at a fair old lick :o

I couldn't answer that without the CAD file of course but generally my approach is to select a modern cutter, look up the manufacturer's data for its feeds and speeds and use these as my starting point in Fusion to program the CAM. These are often a lot more aggressive than I'd have guessed and with a bit of testing you can get a feel for what you can actually achieve on your machine. Some of the modern cutters and inserts are significantly better than those of a decade or so ago, so it's worth trying a few out. They are often less prone to chatter and give higher removal rates (MMRs), lower cutting forces and better surface finishes. Generally I do a roughing operation followed by a finishing operation, rather than one single pass.

Currently Fusion doesn't report the spindle power required to support the resulting feeds and speeds so sometimes I've checked it won't exceed the available power by using one of the tool apps from Iscar, Sandvik etc. I believe Fusion will soon include an estimate of spindle power, so that extra step won't be needed soon. However, although I have only(?) 3kW available, that's enough for some pretty decent MMRs.

I always try to use as much of the flute length as possible, which is made easier by these modern adaptive toolpaths. It evens out tool wear and makes best use of adaptive toolpaths. My "big" machine is from the 1980s and cost as much as a house back then but the toolpaths at the time were very basic, manually coded rectilinear and circular things, whereas modern toolpaths can essentially follow almost any locus. The result is that the machine is now much more versatile and able to much achieve greater MMRs with less risk of breakage than it could previously. The original owner would be pretty surprised to see what it can do now!

To answer your question, once the part is programmed into Fusion CAM, the simulation gives a pretty accurate machining time estimate. In practice I find any significant difference is due to my manual tool changes rather than the machining itself.

One thing I learned fairly early on is the need to clear the (aluminium) swarf from the cutting zone to avoid it being "recut" when achieving high MMRs. Recutting can result in an inconsistent surface finish but above all it leads to the risk of swarf becoming welded to the cutter (ping!). Air and/or high flow coolant is the best way to avoid it!

Murray

Offline kvom

  • Full Member
  • ****
  • Posts: 2031
Re: Going over to the dark (CNC) side!
« Reply #61 on: March 09, 2019, 03:43:58 PM »
I myself tend to be conservative with feeds and speeds as very few parts I make as a hobbyist are critical as to machining time.  A production shop may well decide to test a cutter to destruction, or at least run with spindle power meter at 100%.

Recently CamBam has added an operation for trochoidal pocketing and profiling, which is quite similar to adaptive paths.  Large depth of cut (use more of the side slutes), small stepover, and higher feeds.  This definitely improves chip clearance when machining aluminum as well.

Offline Vixen

  • Full Member
  • ****
  • Posts: 1327
  • Hampshire UK
Re: Going over to the dark (CNC) side!
« Reply #62 on: March 09, 2019, 09:30:50 PM »

Recently CamBam has added an operation for trochoidal pocketing and profiling, which is quite similar to adaptive paths. 

Hi Kvom,

I am considering changing over to CanBam. The latest documented issue, available over here in the UK, appears to be Issue 0.9.8 which does not appear to offer trochoidal pocketing. Can you tell me which version of CamBam I should be looking for which includes the trochoidal pocketing or whether it is an external add-on produced by an outsider.

Thanks

Mike
It is the journey that matters, not the destination

Offline kvom

  • Full Member
  • ****
  • Posts: 2031
Re: Going over to the dark (CNC) side!
« Reply #63 on: March 09, 2019, 10:31:41 PM »
The latest is v1.0 "CamBam Plus".  While is says it's developmental, the reality is that most long term users have moved over from .9.8.  Trochoidal pocking and profiling were added by a user, and work quite well.

It is installed in the base product by copying the trochomops.dll to the Plugins directory.

The trochoidal profile and pocket DLL is available for both versions

Offline Vixen

  • Full Member
  • ****
  • Posts: 1327
  • Hampshire UK
Re: Going over to the dark (CNC) side!
« Reply #64 on: March 09, 2019, 11:13:45 PM »
Thanks for the advise to use issue V1.0 of CamBam and how to add the trochomops.dll to the Plugins directory. I will certainly give that a try.

In the mean time, do you have a copy of a small trochoidal pocket G-code file that I could use to test my Emco F1 mill? That would give me confidence in my machine's ability to cope with this type of high speed machining.

Thanks again for your help

Mike
It is the journey that matters, not the destination

Offline kvom

  • Full Member
  • ****
  • Posts: 2031
Re: Going over to the dark (CNC) side!
« Reply #65 on: March 10, 2019, 12:43:49 AM »
Attaching the .nc file.  The pocket is 50mm square centered on 0,0, 5mm deep.  Tool is 1/4" (6.35mm) endmill.  Roughing clearance 1mm.

Toolpath is plunge to 5mm, then spiral out with a .2 stepover until the sides are reached,  Then each corner is milled with arcs of decreasing diameter.  I didn't know what material or tool, so feeds are notional.  You can do a global replace with appropriate values.  Here I specified only climb milling, so each arc is followed by a G1 to the start point of the next arc.  The program does allow bi-directional arcs, but I usually do it this way to allow chip clearance in aluminum.

If you'd like a better test, provide a DXF/tool spec/meterial and I can easily generate it.

FWIW, all of the aluminum pieces of the hummingbird were machined this way.

Offline Vixen

  • Full Member
  • ****
  • Posts: 1327
  • Hampshire UK
Re: Going over to the dark (CNC) side!
« Reply #66 on: March 10, 2019, 01:00:50 PM »
Due to our time zone differences, your trochoidal tool path file arrived overnight. I only got to play with it after all the mornings household chores were done.

My Mill runs under LinuxCNC control and is set up to machine in inches. Your toolpath are in metric units. I thought that could be a problem but fortunately LinuxCNC recognised the G21 (metric units) and made all the necessary conversions to inch measurements and displayed the trochoidal toolpaths accordingly. That's another first; something else learned.

I pressed the 'RUN' button with some trepidation and off went the machine. The spindle ramped up mto 4,000 rpm and machined air at a feed rate of 24"/ min (600mm/min). All appears to be working well, my mill can handle the feed rates and acceleration in both axes without apparent problem. However, the speed at which the tool moves arround is staggeringly fast, many times faster than I have ever machined anything before. That will take a bit of getting used to. The next thing is to try machining some metal.

Before I can do that, could you please generate a smaller test program, so that I can use the cutters and stock material I have available in the shop. I do not yet know how to attach a file to these posts, so I will have to use words instead. Please could you generate the tool path to make a rectangular pocket, again with 0,0 in the centre, measuring 20mm x 30mm and 6mm deep in aluminium, with a HSS, 5mm diameter three flute end cutting tool. My machine can go to 6000 RPM. I have air blast to clear the chips but no pumped coolant other than a can of WD40

Feeds and speeds must be critical to this high speed machining. What feed and speed calculator do you use? How close to maximum theoretical do you need to run the feeds? Is it OK to slow the feeds down or does that upset the way this high speed machining works?

Thanks again for your support

Mike

BTW.   my petite Colibri hummingbirds built a nest and laid some acrylic eggs.





It is the journey that matters, not the destination

Offline jadge

  • Full Member
  • ****
  • Posts: 370
  • Cambridge, UK
Re: Going over to the dark (CNC) side!
« Reply #67 on: March 10, 2019, 01:49:02 PM »
High speed machining is a bit of a misnomer. It would be better to call the toolpaths constant engagement. To machine a pocket with a conventional rectangular toolpath at each step the cutter has to move across to the next path potentially at full width. So the DOC, and feeds, need to take that into account, despite the linear cutting being done at less than full width. The idea of the high speed paths is that the tool moves so as to keep the cutter engagement constant. Thus DOC, WOC and feeds can be set for those parameters, which are used for the whole machining cycle.

The term high speed machining really relates to maximising the metal removal rate by keeping the cutting parameters constant. It doesn't inherently imply running the cutter at high spindle speeds and feeds. Although of course that would normally be done in a commercial environment to minimise time. Any high speed toolpath will run perfectly well with slow speeds and feeds.

Andrew

Offline Vixen

  • Full Member
  • ****
  • Posts: 1327
  • Hampshire UK
Re: Going over to the dark (CNC) side!
« Reply #68 on: March 10, 2019, 02:38:33 PM »
Andrew,

Thanks for you excellent explanation. The concept of constant engagement toolpaths now make perfect sense. The knowledge that a high speed toolpath will run perfectly well with slower speeds and feeds is very reassuring. I guess the wear and tear on the machinery will also be considerably reduced at the lower rates.

It looks like the high speed, Trochoidal pocketing and profiling plug-ins to CaBam will be very useful addition.

Mike
It is the journey that matters, not the destination

Offline kvom

  • Full Member
  • ****
  • Posts: 2031
Re: Going over to the dark (CNC) side!
« Reply #69 on: March 10, 2019, 04:00:43 PM »
Attached file as per your request.  I use G-Wizard for feed and speed.  I specified 20mm stickout and 50% roughing as additional inputs.  So feed rate is conservative.  Deflection of the tool is .01mm or 56% of breaking point.  Power is .038 kw, mrr 4.33 cc/min, estimated machining time 1:06.

The CB implementation doesn't allow for the non-cutting chords between slices to be generated as rapids, so I chose 1000mm/min arbitrarily.  You could do a global change of the g-code to reduce the speed or to replace G1 F1000.0 with G0.

Offline Jasonb

  • Full Member
  • *****
  • Posts: 6682
  • Surrey, UK
Re: Going over to the dark (CNC) side!
« Reply #70 on: March 10, 2019, 04:38:26 PM »
Thanks for the detail answer Murray and all the other posts which have been interesting to read. I have not had a chance to play with the KX3 this week (see Allman thread)  but hope to get some time soon.

J

Offline Vixen

  • Full Member
  • ****
  • Posts: 1327
  • Hampshire UK
Re: Going over to the dark (CNC) side!
« Reply #71 on: March 10, 2019, 04:53:03 PM »
Kvom, thanks for all your help and support,

66 seconds to demolish all that material...........and you say you have used a conservative feed rate!!!!!!!!

Off out to the workshop to try it for real :noidea:

Thanks again

Mike
It is the journey that matters, not the destination

Offline Vixen

  • Full Member
  • ****
  • Posts: 1327
  • Hampshire UK
Re: Going over to the dark (CNC) side!
« Reply #72 on: March 10, 2019, 05:53:02 PM »
Kvom,

I found I could only command the spindle to 5,400 RPM, so I slowed the feed rate to 80% to compensate.

I have never seen chips fly so fast and so far.

With is Trochoidal milling strategy, I can now achieve the same (once seemingly impossible feeds and speeds and MMR) as Andrew

Thanks

Mike
« Last Edit: March 10, 2019, 06:23:03 PM by Vixen »
It is the journey that matters, not the destination

Offline fumopuc

  • Full Member
  • ****
  • Posts: 2397
  • Munich, Germany, EU
Re: Going over to the dark (CNC) side!
« Reply #73 on: March 11, 2019, 01:11:24 PM »
Hi Jason, I am following your learning curve with the Sieg CNC milling machine with great interest.
I have seen that you are using Vetric software for your first steps. This was also my first choice in 2013, when I have entered the dark side.
In April 2017 I have started the Fusion 360 adventure.
My regular process during the Fusion CAD learning curve was:
Creating a 3D model in Fusion followed by creating a DXF export for the CNC operation.
Importing the dxf file into the Vetric software and getting the toolpathes there.
At the end a very complicated process, but due to laziness or " I have done it always like this" I have used this process until end of November last year.
In my Christmas holidays I took the opportunity and tried the CAM Modul in Fusion360 seriously.
After doing the first parts, I have quickly recognized, that there is a huge and comfortable tool hidden behind this  "CAM" button in Fusion360.
So every possible minute was used to follow some Fusion360 CAM tutorials for learning.
The current status at this issue is, that since beginning of December 2018 my Vetric software is hidden in a dusty corner of my hard disc and I am afraid it will stay there for longer.
Finally is there only the question for me, why does it took so much time to find this way ?
« Last Edit: March 11, 2019, 01:19:21 PM by fumopuc »
Kind Regards
Achim

Offline kvom

  • Full Member
  • ****
  • Posts: 2031
Re: Going over to the dark (CNC) side!
« Reply #74 on: March 11, 2019, 02:29:58 PM »
For someone who uses F360, the built-in CAM makes a lot of sense. 

I use Solidworks which I get for free as a veteran, but the CAM packages that integrate with it are from 3rd parties and not free.  For that reason I use CamBam, which is relatively cheap for a lifetime license and which I find intuitive to use.  I still do the DXF export/import, but it's not overly complex.