By continuing to use this site, you agree to our use of cookies. Find out more
Forum sponsored by:
Forum sponsored by Allendale Jan 24th

Further Adventures with the Sieg KX3 & KX1

A thread for new owners of these machines to post in.

All Topics | Latest Posts

Search for:  in Thread Title in  
Andrew Johnston10/04/2019 11:27:45
avatar
5520 forum posts
648 photos

In my early days of CNC I started off by touching off each tool and noting the offset. However, that got tedious rather quickly, especially when I forgot to type in the offset when changing tools.

I now use a master tool and an electronic tool height setter. The master tool (tool 0) is simply a length of silver steel with a rounded end, on the left in this picture:

cnc_tooling.jpg

The sequence is:

  • Touch off the master tool on the table and zero Z
  • Use the electronic tool height gauge to measure each tool against the master tool and automatically fill the tool table. Measuring each tool is a one button push on the screen
  • Touch off the master tool on the fixture or work, depending upon where the zero height reference was set in CAM
  • Set X & Y zeros
  • Start machining!

Andrew

Ian Johnson 110/04/2019 12:08:47
271 forum posts
81 photos
Posted by Andrew Johnston on 10/04/2019 11:27:45:

In my early days of CNC I started off by touching off each tool and noting the offset. However, that got tedious rather quickly, especially when I forgot to type in the offset when changing tools.

I now use a master tool and an electronic tool height setter. The master tool (tool 0) is simply a length of silver steel with a rounded end, on the left in this picture:

cnc_tooling.jpg

The sequence is:

  • Touch off the master tool on the table and zero Z
  • Use the electronic tool height gauge to measure each tool against the master tool and automatically fill the tool table. Measuring each tool is a one button push on the screen
  • Touch off the master tool on the fixture or work, depending upon where the zero height reference was set in CAM
  • Set X & Y zeros
  • Start machining!

Andrew

I like that method Andrew, usually I take the Z offset from the longest tool, but having one dedicated master tool is a good idea. The only problem I can see is a restriction on Z height on my KX1. Are you using Path Pilot they look like Tormach tool holders?

Ian

John Haine10/04/2019 15:10:05
3109 forum posts
162 photos

Andrew, do you touch off the master tool on the table or the height setter? Presumably the latter if the heights of the other tools are measured using the setter? Is your master tool solid or is the tip isolated?

Andrew Johnston10/04/2019 15:35:38
avatar
5520 forum posts
648 photos
Posted by Ian Johnson 1 on 10/04/2019 12:08:47:
Are you using Path Pilot they look like Tormach tool holders?

I am indeed using PathPilot and the toolholders are Tormach, although I use them on the Bridgeport as well.

The concept of tool 0 came from a professional CNC book. One advantage is that the master tool is longer than most real tools so less chance of a crash. But of course it's bad if you have limited Z. Tormach now advise using the spindle nose as a reference. In theory that should be "slightly" more accurate as one is removing one variable, the interface between the toolholder and spindle nose. But in practice it's a PITA as the spindle nose is large, you can't see what's going on and it's no good for recessed reference planes. So I've stuck with a master tool.

Andrew

Andrew Johnston10/04/2019 15:40:54
avatar
5520 forum posts
648 photos
Posted by John Haine on 10/04/2019 15:10:05:

Andrew, do you touch off the master tool on the table or the height setter? Presumably the latter if the heights of the other tools are measured using the setter? Is your master tool solid or is the tip isolated?

I touch off on the table. The electronic tool height setter is from Tormach and is integrated into the software. So the system knows that the tool setter is 80mm high and takes that into account automatically. The master tool is solid, no electronics involved. I simply ramp down slowly until a fag paper is trapped.

Andrew

Emgee10/04/2019 17:34:27
1500 forum posts
218 photos

My method is old hat but doesn't require special tools or programs, just enter the tool offset in the toolchange line in the program,

**LINK**

Emgee

Ron Laden10/04/2019 19:16:11
avatar
1942 forum posts
384 photos

Thanks guys, one more question: when a job is running is it possible to adjust the tool speed and feed rate or does the job have to stop to re-visit whats programmed.

JasonB10/04/2019 19:19:23
avatar
Moderator
18157 forum posts
1998 photos
1 articles

Mach3 allows you to override feed in 10% steps and speed can also be overridden both while the machine is running using the up and down arrows in the two boxes bottom right

20190222_074804.jpg

Edited By JasonB on 10/04/2019 19:20:55

Andrew Johnston11/04/2019 09:36:17
avatar
5520 forum posts
648 photos
Posted by Ron Laden on 10/04/2019 19:16:11:

Thanks guys, one more question: when a job is running is it possible to adjust the tool speed and feed rate or does the job have to stop to re-visit whats programmed.

Yes, but I've never used the facility. One might do an aircut at slower speed if clearance on clamps, for instance, is tight. But once a program is cutting metal let it get on with it. Unlike manual milling you make a decision as to speeds and feeds and let the program run. And then go and do something else. For CNC milling you need a better understanding of speeds, feeds, widths and depths of cut than for manual milling. Which is why the "all you do is press a button" brigade are wrong. smile

Andrew

John Haine11/04/2019 12:36:00
3109 forum posts
162 photos

I tend to be a bit wimpish with feeds and often find myself turning the feed up once a cut has started when it's evident that it's too slow.

JasonB13/04/2019 12:18:13
avatar
Moderator
18157 forum posts
1998 photos
1 articles

The adventure continues with this part which will be the bottom mounting flange of the cylinder.

cylinder base.jpg

First operation was to run the code which put the four 3mm holes into an oversize piece of 1/4" flat steel bar. I then put an offcut of aluminium into the vice and ran the code again but this time with a 2.5mm drill, the holes were then hand tapped and the two screwed together without removing the aluminium tooling plate from the vice.

With a 6mm dia 3-flute carbide cutter I first ran an adaptive clearing cut around the outside followed but a final contouring cut to finished size. I started off quite tame at 3000rpm and 150mm/min feed but found that could be upped as the flat bar cut a lot better than the steel plate I was cutting the other day.

The next part of the code had the adaptive clearing to form the 4 raised bosses, this again had been programmed as above but found I could go faster and ended up at 3900rpm and 225mm/min feed.

Again Youtube has added some high frequency noise but you can see the first cut around the outside where the DOC varies as I only rough centered the work followed by 3 clips of the top clearing at various stages.

Final job was to skim the bottom off, final size will be done after silver soldering the assembly together.
20190413_104654.jpg
Intention is to have a 20mm block between the bosses so a quick test with an ARC 10-20-40 block to see what the fit is like
20190413_104914.jpg
Can't get much better than this
20190413_104925.jpg
Ron Laden14/04/2019 08:29:00
avatar
1942 forum posts
384 photos

Looking good Jason I will have to admit my ignorance though...adaptive clearing cuts...?

Ron

Barrie Lever14/04/2019 09:38:01
599 forum posts
61 photos

Spiral approch adaptive roughingRon

Adaptive clearing/roughing

Take a normal simple pocket operation, at some stage the cutter is going to need to cut at its full width, so to allow for this max strain upon the cutter and machine, you either have to set the DOC lower and maybe make two passes or run slower than ideal.

The same pocket with adaptive clearing would be approached with a spiral entry into the work piece creating a hole somewhat bigger than the cutter diameter. Generally step over tends to be smaller with adaptive strategies, you can see that Jason was using probably a 15-20% step over (maybe 1mm) on the 6mm cutter. So the tool never sees the load of the full width (6mm in this case). Maybe you can see what I am describing in the screen shot, this was for a carbon fibre machining job (very abrasive !!).

This allows you to use the side flutes of the cutter more effectively rather than stepping down in a number of passes, tool life is extended by some margin. You can also run hobby machines closer to industrial feed rates albeit with smaller stepovers.

Some adaptive strategies allow climb and conventional milling in the same tool path, so in this case the tool would have zig-zagged backwards and forwards.

You would think this would always be an advantage but not so, particularly if the cuts are long it is quicker to rapid back to the start. I think in Jason's example though zig-zag (climb/conventional) would get material off quicker.

Modern CNC machining (HSM) seems to be favouring taking lighter cuts on the side of the tool and with very high feed rates. Rather than old manual techniques which I think tended to go for big stepovers.

If I followed Jason's reports more closely I would see what CAM package he is using, of course the package may not have adaptive zig/zag.

B.

Edited By Barrie Lever on 14/04/2019 09:39:13

Edited By Barrie Lever on 14/04/2019 09:41:45

Edited By Barrie Lever on 14/04/2019 09:48:48

Edited By Barrie Lever on 14/04/2019 09:50:33

Andrew Johnston14/04/2019 10:08:50
avatar
5520 forum posts
648 photos
Posted by Barrie Lever on 14/04/2019 09:38:01:

Modern CNC machining (HSM) seems to be favouring taking lighter cuts on the side of the tool and with very high feed rates. Rather than old manual techniques which I think tended to go for big stepovers.

That's a pretty good summary. Took me quite a while to realise I was better off running fast with small cutters on the CNC mill rather than trying to hog out with large cutters at slow speed.

In the video the tool seems to spend an inordinate time cutting air. I suspect a climb mill only button has been selected? I normailly use climb milling for a finishing cut but for roughing out I select both, so you get the zig-zag cutting.

Andrew

JasonB14/04/2019 10:35:50
avatar
Moderator
18157 forum posts
1998 photos
1 articles

Thanks for the explanation Barry and also to Andrew for his input.

From posting on another forum I have found out that I had the return movements set the same as the cutting feed which slowed things down quite a lot.

After reading your replys I have looked and found where I can set the tool to cut in normal, climb or both directions and changing to both has again reduced the time according to the simulator. I had just been using climb cutting.

For Ron these are screen shots of the simulator, the blue line represents the axis of the spindle and you can see that the tool steps over 1.5mm for each pass which is what I was doing in the video. The yellow lines ae where the tool returns to the start of a cut so time wasted

cylinder base adaptive.jpg

This screen shot is with the cutter set to cut both ways so less time not removing metal on the return movements, blue in climb cutting, yellow conventional direction.

cylinder base adaptive both ways.jpg

Edited By JasonB on 14/04/2019 10:36:45

Ron Laden14/04/2019 11:20:55
avatar
1942 forum posts
384 photos

Thanks guys , interesting stuff.

Ron

Ian Johnson 114/04/2019 15:00:31
271 forum posts
81 photos

Good explanation of adaptive machining thanks Barrie. I am using Vectric Vcarve and don't think they have an adaptive strategy, unless I'm not looking hard enough?

And I too have also come to the conclusion that small cutters and more faster cuts are the best way to tackle CNC milling, less stress on the machine, especially on a little hobby mill. Apart from a fly cutter and edge finder, I very rarely use any cutter over 6mm dia now, there is no need to!

Ian

JasonB16/04/2019 19:07:31
avatar
Moderator
18157 forum posts
1998 photos
1 articles

To finish the sandwich construction of the engine base some form of filling was needed and as I have quite a few off cuts of Corian I decided to use that rather than metal.

The sequence was much the same as the top and bottom plates but I tried out peck drilling for the 3mm holes as they were quite a bit deeper than before, I could have gone faster with the retract speed and not lifted so far out of the work, drill was running at 5000rpm.

I used a chip breaker feed for the larger holes, you can't see it that well on the video but can hear when the drill pauses the feed which if I was drilling steel or Ali would shorten the swarf, dropped down to 1000rpm on the 6mm and 7.8mm holes.

Finally machining the contour where you can see the tool ramp down and then start cutting in 2mm deep passes before it starts to get lost in the swarf which is when I stopped filiming and got the vacuum running. The 3-flute Carbide cutter romped through this at 5000rpm and 350mm/min feed.

I did not use any tabs this time as the material was thicker than needed, bottom milled off afterwards.
m3.jpg
Quite pleased with the cut edge, no sign of cutter marks when held upto the light, this was a full depth finishing pass
m4.jpg
I used a 50mm face cutter to thin the work down to 10mm moving the clamps to complete the ends, only downside to working with Corian is the mess.
m1.jpg
m2.jpg
I'll bond it all together with JB Weld but that won't be until the bearing supports have been fabricated and silver soldered to the top plate but could not resist a quick trial assembly.
m7.jpg
m5.jpg
m6.jpg
Ian Johnson 116/04/2019 23:35:14
271 forum posts
81 photos

It's coming together nicely Jason. Good idea to use Corian as a filler, I don't suppose it matters what its made of, as long as it does the job and looks good when finished.

Had to Google Corian, never used it before, looks like good stuff. Messy though!

Ian

John Haine17/04/2019 07:26:42
3109 forum posts
162 photos

I'm sure you've said somewhere Jason, but what CAM program do you use please?

All Topics | Latest Posts

Please login to post a reply.

Magazine Locator

Want the latest issue of Model Engineer or Model Engineers' Workshop? Use our magazine locator links to find your nearest stockist!

Find Model Engineer & Model Engineers' Workshop

Support Our Partners
ChesterUK
EngineDIY
Allendale Electronics
cowells
Warco
emcomachinetools
Eccentric July 5 2018
Eccentric Engineering
Subscription Offer

Latest "For Sale" Ads
Latest "Wanted" Ads
Get In Touch!

Do you want to contact the Model Engineer and Model Engineers' Workshop team?

You can contact us by phone, mail or email about the magazines including becoming a contributor, submitting reader's letters or making queries about articles. You can also get in touch about this website, advertising or other general issues.

Click THIS LINK for full contact details.

For subscription issues please see THIS LINK.

Digital Back Issues

Social Media online

'Like' us on Facebook
Follow us on Facebook

Follow us on Twitter
 Twitter Logo

Pin us on Pinterest