Joe's 1000x600x200 steel and aluminium router started

[JAZZCNC]

Those look excellent value thanks. How deep DOC do you go with the rougher in ali?

It depends on the grade. I mostly use Cast tooling plate and I can take 4mm DOC slot milling with coolant but I often keep it to half that with a bump in feed to save the cutter but run it dry with air. to keep the mess down. Feeds n speeds I tend to play around with depending on the job but they range from 1000mm/min to 1600mm/min. RPM 12K to 20K often around 15k.

I did play around with deeper DOC and the cutters will happily take 100% Dia but my 2.2Kw spindle isn't very keen, there's nothing left for a safety margin and a slight soft spot will stall it.
Side cutting it will happily take 1.5xD and I often cut 20mm plate full pass just dibbling it away 0.30mm, which is roughly the serration depth, hence my 0.4 finish passes. When using i-machining (adaptive) I can really ramp it up and it's crazy fast at full DOC.

[devmonkey]

It depends on the grade. I mostly use Cast tooling plate and I can take 4mm DOC slot milling with coolant but I often keep it to half that with a bump in feed to save the cutter but run it dry with air. to keep the mess down. Feeds n speeds I tend to play around with depending on the job but they range from 1000mm/min to 1600mm/min. RPM 12K to 20K often around 15k.

I did play around with deeper DOC and the cutters will happily take 100% Dia but my 2.2Kw spindle isn't very keen, there's nothing left for a safety margin and a slight soft spot will stall it.
Side cutting it will happily take 1.5xD and I often cut 20mm plate full pass just dibbling it away 0.30mm, which is roughly the serration depth, hence my 0.4 finish passes. When using i-machining (adaptive) I can really ramp it up and it's crazy fast at full DOC.

Right i'll order a couple, sounds excellent. Are you saying you can cut cast plate full depth (20mm) at 1000mm/min using trochoidal/adaptive? I haven't tried anything like that aggressive, I usually cut at 6mm DOC with a 6mm cutter, ~1600mm/min and 1mm stepover into plate with trochoidal.

[JAZZCNC]

Right i'll order a couple, sounds excellent. Are you saying you can cut cast plate full depth (20mm) at 1000mm/min using trochoidal/adaptive? I haven't tried anything like that aggressive, I usually cut at 6mm DOC with a 6mm cutter, ~1600mm/min and 1mm stepover into plate with trochoidal.

No Using i-machining which is Solid-Cam's version of trochoidal I can cut much more aggressively than 1000mm/min at 20mm DOC. i-machining adjusts the feed based on geometry while it's cutting and usually, it's anywhere between 2000-4000mm/min and 14-18000rpm. And that's on the medium setting 4, if I bump up the level to 7 it really rips chips, but it knocks the hell out the machine and spindle so I keep it between 3-4. This usually spits out feeds between 2-3000mm/min, 12000rpm and varies the step over between 0.1 and 0.9mm. See Pic

[szecho]

I have read this thread and I have a question.
I saw you have plates welded on the frame and a washers under the supports.
How did you position the ball screw support (bk/bf) on the frame? By the thickness of the washers you set the screw to be parallel with the rail?

[Tom J]

Hi
Is it SKU IR26526 profile?

No delete option for duplicate post - sorry:(

[Tom J]

Gantry extrusion has arrived from KJN, it is a real beast. KJN cutting appears very accurate.

Attachment 26902 Attachment 26903

So now I need to decide how to mount 15mm rail to the extrusion. I was considering 3 options:
1. Mount rail directly to extrusion between the two slots, drilling and tapping.
2. Mount rail on aluminium plate which is in turn bolted to the slots.
3. Mount rail directly to slot.

This shows that the profile is not flat across the width which I believe is by design so that the slots pull up to meet whatever you are clamping to them. The slot edges are 0.15mm lower than the centre, the centre and the 2 corners are perfectly aligned within the resolution I can measure with finest feeler gauge.

Attachment 26905

Now I have the extrusion (1) is a non-starter as there is a very slight peak in the centre and I would need to mill it flat which is hard given the gantry is longer than my mill table, although not impossible.
(2) is what many people seem to do and so obviously works but is more work for me.
Can I get away with (3), see picture below, what do you think?

Attachment 26904

I have a 50mm fly cutter, it would be possible given the extrusion is already flat and parallel to fly cut between the high points, would have to tram the mill carefully first.

Hi
Is it SKU IR26526 profile?

[devmonkey]

Making some minor improvements to my machine so thought I'd report them here.

I've been using an mdf spoil board with t-nuts, I have hated this solution from the beginning but have been avoiding tapping 250 M6 holes in the alu bed plate.

I decided to just do it, I wasn't going to tap them by hand so I purchased a thread cutter for M6. The bed is made of 20mm cast aluminium plate, since there was only one chance to get this right I tested all the feeds and speeds on some scrap identical plate first. This was the first time I have used a thread cutter and you must dial in the toolpath first to get the type of fit you want on the bolt (basically change the diameter by 5 microns until happy). I'll give some details of the feeds and speeds to help anyone else processing similar material with a 2.2kw chinese spindle on a job that cannot be messed up.

1. Drilling was the main concern with the chinese spindle as it has not much torque at the rpm drill bits need. I found the sweet spot to be the spindle slowed down to 5300 rpm, feed rate 700mm/min, 2 pecks each half depth to total depth of 19mm. Less rpm or more feed and spindle would stall, more rpm or less feed and chips would melt on the tip.

Sprayed some WD40 on it for each hole. This created nice shiny round holes, bit was still like new afterwards, not bad for something that probably cost a few pence.



2. Chamfered with a 6mm 45 degree bit.

3. I blew out the holes, then sprayed WD40 over each.

4. Thread cut bottom up with this bit at 16000rpm 250mm/min:
https://www.shop-apt.co.uk/metric-si...60480N1.0.html





Result was a perfect grid of blind tapped holes on 50mm pitch, very pleased.

[devmonkey]

New spoil board machined with thru holes to reach the threaded bed holes. Missing corner is for vice and 4th axis which sit on their own registration plates. Sometimes I need to cut jobs that use the whole bed, when I next need to do one i'll make another spoil board without the missing corner, they only take a few minutes to swap and surface.

Next improvement will be replacing the standalone ddnc 3.1 controller with UCCNC and their ethernet motion controller. I need the ability to write custom plugins / macros which is missing / hard with the ddnc.

Does anyone know if there is stock of these in the UK, I vaguely remember someone, Jazz?, may have been a distributor?

[Clive S]

New spoil board machined with thru holes to reach the threaded bed holes. Missing corner is for vice and 4th axis which sit on their own registration plates. Sometimes I need to cut jobs that use the whole bed, when I next need to do one i'll make another spoil board without the missing corner, they only take a few minutes to swap and surface.

Next improvement will be replacing the standalone ddnc 3.1 controller with UCCNC and their ethernet motion controller. I need the ability to write custom plugins / macros which is missing / hard with the ddnc.

Does anyone know if there is stock of these in the UK, I vaguely remember someone, Jazz?, may have been a distributor?

Yes. Jazzcnc is a member of this forum. https://www.jazzcnc.co.uk/