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  
Nicola Casali22/05/2021 15:59:09
33 forum posts
6 photos

Sorry, I was referring to https://youtu.be/HWVk5nqtSXc

I just realised I used F360 for the flanges. I may have attempted Aspire first. The stock is 6.35mm. I was using a 1mm stepdown with a 4 flute endmill. I'll try your suggestions, as I need to make 3 more. Great!

 

Edited By Nicola Casali on 22/05/2021 16:00:45

JasonB22/05/2021 16:08:20
avatar
Moderator
21613 forum posts
2490 photos
1 articles

Ah that was one of the first things that I did when I got the KX3 and was still learning. This one from from a couple of months ago has a 4mm cutter moving at 300mm/min twice the speed of that 6mm one.

Nicola Casali22/05/2021 16:16:44
33 forum posts
6 photos

I've tried tabs, but got some nasty vibrations with my non-centre cutting endmills. I don't think it's ramping into those tabs, for some reason. I tried triangular ones.

Edited By Nicola Casali on 22/05/2021 16:17:48

JasonB22/05/2021 16:22:50
avatar
Moderator
21613 forum posts
2490 photos
1 articles

Thats another reason for doing it the way I tend to as the tabs can cause a bit of chatter and are the limiting factor when it come sto feed though the triangular ones are better and ramp speed can be set to less than cutting speed.

You should be able to do your parts the full 1/4" depth with 0.75 to 1mm stepover on the 2D adaptive, say 4500rpm and 300mm/min if 3-flute, 400mm/min if 4 flute. You can always over ride the speed if it sounds happy and try a bit faster

JasonB23/05/2021 17:16:33
avatar
Moderator
21613 forum posts
2490 photos
1 articles

With another member making tentative steps towards CNC cutting a conrod and recent talk of adaptive and contour cuts I made this video of this mornings efforts.

It's the conrod for the 11cc Wall engine I have been working on, some manual work had already been done machining up the two halves bolting together which also entailed reducing the rod width so that counterbored could be drilled for the cap head screws which have to go in from the small end and the two holes had also been drilled and reamed.

When doing the CAM I also picked up on the two diameters and used them to locate some holes to drill the scrap used to hold the part at the correct spacing and subsequently tapped these by hand with a 3mm spiral flute tap. Using some top hat bushes the blank was secured ready for machining.

First an adaptive to remove the majority of the waste then a contour to do the outer shape. Followed this with a radius corner cutter to form the two bosses and then a 3mm ball nose for the recess in the side of the rod. at 6.08 in you can hear the sound of the cut change as a bit of ali welded onto the tool as it took a full width cut so a quick reduction in feed and a dab more paraffin just managed to save the day, the other side cut fine using the slower rate from the start. Full details of cutters/feeds/DOC etc in video description.

JasonB16/10/2021 19:01:23
avatar
Moderator
21613 forum posts
2490 photos
1 articles

One of the members of MEM forum has just upgraded his machine to a 1.1Kw teknomotor HFspindle and posted some test cuts with it, I queried the 18,000rpm that he was running the HSS cutter at and an interesting discussion about HSS/Carbide and various feeds and cuts followed. You will need to register to see most of the images which are posted as attachments if you are not already a member

This lead me to sacrifice a bit of 6082 to see how quickly I could convert it into a pile of chips.

As I have mentioned before I tend to use 3-flute cutters most of the time so this was no exception and I chose an Aluminium specific one from APT with a 55degree Helix that had had some but not too much use.

They give some suggested parameters for side cutting of 13,000rpm and 1,500mm/min feed so working that back to my maximum spindle speed of 5000rpm gives a feed of 577mm/min. They don't give how large the side cut can be but most other makers seem to suggest an Ae (sideways feed) of 0.1 D so I went with this making each pass 0.6mm. Ap (vertical Depth) of side cutting seem to either be given at 1D or 1.5D so I went half way with 1.25D which equates to 7.5mm. I drew up a simple block 2" (51mm) wide with a 0.6 x 7.5mm rebate in it and produced the code to cut that at various Fz (chip load) values and simply altered my Y axis zero by 0.6mm each time to compensate for the previous cut. Once I got to 500mm/min I just used the override to increase in steps of 20% eg 100mm/min.

For the first few cuts I just dabbed on a bit of paraffin but for the 800m/min and above also turned on the air as I was having problems getting the fluid to flow with the air. and being an external cut the chips were doing a reasonable job of staying away from the cutter anyway.

At no time did the machine seem to be under any strain, there was a bit of vibration on the 450mm/min pass but that was from the chip guard rather than the cutter. I stopped at 1000mm/min as I did not want to push too much and risk metal welding to the cutter or worse. Even at the highest feed the finish was quite good for what is a roughing cut with a fine series of vertical lines that could be seen when held to the light but not felt with a finger nail.

I'm not sure how often I will run at 1000mm/min as it will depend on the job as to any increases in cutter engagement or getting the chips out if a small pocket is being cut but it is nice to know what the machine can handle.

I put video and an image of the cut surface together with the feed rate son a video, couple are not the best for focus and I also mucked up the 600 & 700 videos but there was nothing exciting to see there anyway.

Ron Laden17/10/2021 10:11:44
avatar
2253 forum posts
446 photos

Wow Jason those feed rates are impressive, at the 1000mm/min blink and you would miss it plus the surface finish looked very good to me.

Ron

Martin Connelly17/10/2021 12:02:08
avatar
1930 forum posts
207 photos

I was trying to cut a simple step with a Little Hogger in some aluminium at 500mm/min and Mach3 detected a fault and stopped. Reset it and tried 400 then 300 then 200 and it kept stopping. Thought something was overloading the machine but finally traced it to a dodgy wire on a limit switch being upset with the vibrations. I fixed it and finally cut the step. The first time you set up something at these high rates makes you a bit twitchy but is satisfying when it works. I have not tried 1000mm/min as I am not sure my top speed is set to go that high.

Martin C

JasonB17/10/2021 13:05:33
avatar
Moderator
21613 forum posts
2490 photos
1 articles

I can understand the vibrations with a little hogger being 2-insert and negative rake, there will be a lot more of an interrupted cut than a 3-flute cutter with the 55deg helix angle as that is engaged in the work for a lot longer per rotation. I've even noticed it of the 2 insert APKT holder.

JasonB27/10/2021 18:23:15
avatar
Moderator
21613 forum posts
2490 photos
1 articles

I had a pressing little job for another forum member that needed cutting from some 20mm thick EN3 steel so thought I would have a play with the feed rates. The cutter is once again a 6mm 3-flute carbide one this time made by New Century which is YG-!'s Chinese factory and it has had quite a lot of previous use on steel and iron. I have attached their speed and feed chart but as the first set of figures is for carbon and alloyed steels upto 1000Nm and I was only cutting a low carbon steel I upped the spindle speed to 5000rpm and also increased Ae (sideways feed) to 0.1D or 0.6mm. Ap (height of cut) was 5.5mm which suited the 20mm thick workpiece giving 4 passes with the tool finishing below the bottom of the work piece.

nc mill.jpg


First pass was at 300mm/min, then using the override which goes up in steps of 10% 450mm/min, then 510mm/min which gave a Fz (chip load) of 0.034mm which it seemed more than happy with and I should think 600mm/min x 6.0mm Ap quite possible but that can be tested on some scrap. At the end of each piece there was no noticeable increase in the temperature of the work and what heat was in the tool was only slight and likely to have come from the spindle rather than the cutting end so looks like the chips were carrying away all the heat as they should. I was cutting dry with no air as chips were getting thrown well clear of the work.

The adaptive cuts were set to leave 0.2mm stock which was removed with a finish pass at 200/min, You can see that the first 5-6mm of the tool that had been worn is leaving a dull finish but as the less used upper flutes make contact they are giving a brighter finish. This is only visual as I can't feel any difference

Can you tell what it is yet?

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

Latest Forum Posts
Support Our Partners
rapid Direct
emcomachinetools
walker midge
cowells
Warco
JD Metals
Eccentric July 5 2018
Eccentric Engineering
Subscription Offer

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