Further Adventures with the Sieg KX3 & KX1

[JasonBModerator @jasonb]

As all the machines that were received or on offer have all gone from ARC Euro Trade I have started this thread to post my learning curve with these machines and hope that the other new owners will post what they are doing too.

J.

[JasonBModerator @jasonb]

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

[JasonBModerator @jasonb]

Well while most of the membership seem to have spent the last few days in the armchair working out what size knurl is needed to go around a propane tank to ensure that it gets a CE stamp I have been playing with the KX3.

It is all well and good cutting random shapes into bits of scrap to get the feel of things but nothing beats making more productive swarf. To this end I have been drawing up the next stationary steam engine for a while and was possibly going to get a couple of the parts laser cut but now that I have the CNC what better way to learn and be productive at the same time. The base "casting" of the engine will be a sandwich of 3 layers so I started with the bottom one, the upper is similar but has some different holes and bosses.

A Step file of the required part was exported out of Alibre and into a CAM program where I generated the G-code for the holes and the actual shape as separate sets of code to make it easier for me rather than have to incorporate tool changes. I air ran the code first of all and then again into some PVC which showed up a slight error in heights which was corrected before cutting metal.

I started by clamping the stock onto some MDF and first ran code for eight 3mm holes, then after changing bits ran another code to enlarge four holes to 6mm. After that these holes were used to screw the 2.5mm thick plate to the MDF so that the clamps could be removed. After changing to a 6mm 3-flute HSS FC-3 cutter the button was pressed. I'm more than happy with what came out for my first proper part using CAM and the first time cutting steel and this plate is a bit gummy.

A couple of areas did not quite cut all the way through which was probably due to the scrap MDF that had been sitting around for a while but that just tore away. You can also see that I left some 1mm thick tabs to stop the larger pieces of waste moving about.

Final item after a quick clean up of the burrs

[Old SchoolParticipant @oldschool]

My day has not been that successful, I have tried to load Mach3 onto a machine running Vista. I know the Sieg manual says it won't work but Mach 3 says it will with the fix. I did the fix lots of reboots but I cannot find the file driver test.exe. Given up until back from hols and I will contact the Mach software people see what they think before buying an XP machine.

[Neil WyattModerator @neilwyatt]

I've just bought an XP desktop machine off the 'bay, complete with screen for £25, but haven't picked it up yet.

Neil

[Old SchoolParticipant @oldschool]

Having read the mach3 forum xp seems the way to go. It must be possible to load xp onto my vista machine a disk is not that expensive on the bay but I am no computer wiz.

[SamsarandaParticipant @samsaranda]

I think Vista may not allow a previous version of Windows to be installed, just a thought, not an expert on windows since I defected to Apple!

Dave W

[JasonBModerator @jasonb]

I also got a recon XP machine and screen off e-bay for £50, thought I would start with a clean slate and it also means you can load the Sieg version of Mach3 which is all setup ready to go rather than try and configure it from scratch.

[The Novice EngineerParticipant @thenoviceengineer]

Posted by Samsaranda on 07/04/2019 17:09:16:

I think Vista may not allow a previous version of Windows to be installed, just a thought, not an expert on windows since I defected to Apple!

Dave W

XP can replace a Vista OS , reformat the partition and do a clean install.

Its one of the options from an XP installation CD when you boot from it

Steve

Edited By The Novice Engineer on 07/04/2019 22:07:39

[Ian Johnson 1Participant @ianjohnson1]

Looking good Jason, thinking of the machining sequence is half the battle with CNC.

I've been trying to get my head around my 4th axis on the KX1 recently, I've hand written a couple of little programs to test it out in Acetal. One was an 18 splined knob, another was a seven sided nut, chamfer on all sides, spot drilled on all sides, and a shoulder was milled into it using the rotary axis. I'm gradually sussing out how much can be done on the 4th axis. The Seven sided nut turned out really good too, using 51.43 degrees gave only 0.01 error.

Ian

[Ron LadenParticipant @ronladen17547]

 

Looking good Jason, are you going to tackle the pair of flywheels from solid, I would have thought the CNC ideal for that type of work.

Ron

Edited By JasonB on 27/04/2019 14:21:47

[JasonBModerator @jasonb]

Ron, I'm still deciding which way to go as they have more detail than the rough sketched ones shown, the spokes are a soft + cross section. May go for slices of CI, separate spoke "disk" with a rim & hub or could even modify a casting to get the spoke profile right.

[Ian Johnson 1Participant @ianjohnson1]

Some info for those just starting out with the KX1/3 I started out running my KX1 on Windows 7 professional in XP mode, and that worked great ….. until the tower PC died!

I am now running my KX1 on Windows 7 32 bit on another tower PC, because at the time I couldn't find a suitable XP system, and so far so good, everything is behaving as it should. After I bought the tower PC I found out that standard Windows 7 cannot be run in XP mode! But all is okay.

Ian

[Ron LadenParticipant @ronladen17547]

Posted by JasonB on 08/04/2019 10:19:15:

Ron, I'm still deciding which way to go as they have more detail than the rough sketched ones shown, the spokes are a soft + cross section. May go for slices of CI, separate spoke "disk" with a rim & hub or could even modify a casting to get the spoke profile right.

Yes I can see if the flywheels have more detail it probably means a different approach as you say. I cant fully see the connecting rod to the crank but it looks "different" I,ve not seen one like that before, it looks like a larger version of the one on the valve gear..?

[JasonBModerator @jasonb]

The conrod and eccentric rod are bot "wishbone" shaped with the crosshead being on a single guide that fits between the fork rather than the more usual pair of crosshead guides that the conrod runs between. It uses split bearings with cotters and wedges which should keep me quiet for a while, similar to the Benson engine I did some time ago.

The two photos that I am working on are here and here, don't have much detail but it is most likely French and carries the makers initials "FD"  or could be Fives Lille. The teardrop shaped hoop will contain a governor that has gone walk about over time.

Edited By JasonB on 08/04/2019 16:44:30

[JasonBModerator @jasonb]

I had a bit of time this afternoon so thought I would do the top plate, I did not air cut this time but did practice on some PVC before cutting metal.

First was to drill 15No 2.5mm holes with a split point stub drill which meant I could get away without spot drilling first

Then a change to a 6mm stub drill to open up six of the holes

Using these holes the plate was screwed down to the MDF below and clamps removed. Using a 6mm dia 3-flute cutter but carbide this time the profile was cut, not a bad finish on the bottom of the first pass.

All complete, the 6mm piloted holes that open out to the edge were enlarged to 8mm as part of the contour cut and I left tabs again to stop the waste flying about.

After a clean up with the bottom plate that I cut at the weekend.

I've stitched two videos together here, the beginning shows the first pass with the cutter at full width but 1mm away from the finished edge, second half shows the final full depth finishing cut, you can see the tool rise and fall where the tabs are located. the Upload to Youtube seems to have added some high pitch noise which was not there at the time.

I could quite get to like this CNC lark, next part has been through the CAM and will let me try some adaptive clearing cuts!

[Ron LadenParticipant @ronladen17547]

Great stuff Jason, I can see the attraction of CNC and it making quite light work of difficult parts or parts that would require a lot of setting up to achieve the various shapes if milled manually.

I have very little understanding of CNC but I do find it fascinating. A question: obviously depth of cut is written into the programme but how do you set up the tool depth position in the first place once the tool is fitted into the collet (if that makes sense)

[John HaineParticipant @johnhaine32865]

Ron, one way is to use a tool height setter that automatically sets the height to a known value.

"Here's one I made earlier". This is a simple gadget with a TC button springloaded to be exactly 38.84 mm above the table, that fixes down with a magnet. The button is electrically isolated and connects to the probe input on the controller – when the tool touches the button "Z" is set to 38.84 and the tool retracts to 50 mm. You can also see in the chuck an edge finder that works in a similar way which can set the controller X and Y zero to the work edges, or find the centre of a hole, with high precision. Sorry the photo is on its side.

[JasonBModerator @jasonb]

Nothing quite so fancy here yet. I have just been using the 20mm edge of an ARC 10-20-40 block to touch off onto and entering the height at +20.

[Martin ConnellyParticipant @martinconnelly55370]

A simple but effective way to set z height is with a ground dowel, 10mm for example. You manually lower the tool to about 9mm above the surface you want to be z=0. You then creep up the z axis until the dowel just fits under the tool and set z=10 (or whatever your dowel is). A bit more time consuming than a tool setting switch but if you have plenty of time but money is tight it is an option.

Martin C

[John HaineParticipant @johnhaine32865]

Tool height setter made from the scrap box, except for one spring and a neodymium ring magnet. Edge finder used a length of 10mm ground stainless from an old printer, one short length of M5 studding, a blob of araldite, and some scrap brass. I started using dowels etc for setting but the speed, convenience and accuracy of even simple methods was a revelation.

[Andrew JohnstonParticipant @andrewjohnston13878]

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:

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 1Participant @ianjohnson1]

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:

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 HaineParticipant @johnhaine32865]

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 JohnstonParticipant @andrewjohnston13878]

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

[Author]

Posts