Very nice gentlemen....I want to be able to do that when I grow up.
Printable View
Very nice gentlemen....I want to be able to do that when I grow up.
Well done, nice bit of work that. BTW, how did you hold it whilst machining? Pieces like that where the finished part doesn't have a lot of thickness I always find a bit of a challenge to hold down rigid.Quote:
Originally Posted by devmonkey
Very nice Kit! This was the first time I'd used trochoidal clearing, definitely a keeper for thin endmills in metal.Quote:
Originally Posted by Kitwn
Now I have a question for you pulley experts. I need to make a very large 157 tooth 8m timing pulley ring that will be fitted to the perimeter of a winch drum. The pulley needs to be made of a ring of material ~25mm thick with an outer diameter of 400mm and inner of 340mm. It could be made from aluminium, SRBP, delrin or even hdpe.
Trouble is I don't want to waste a large piece of material just to make the ring, any ideas? I've even considered casting a blank in aluminium but I don't have a foundry. Are there any castable machineable urethanes that are strong enough for timing belt pulley teeth?
I'm well pleased with the trocho pocket plug-in, it's a major step forward in being able to make hardwood clock wheels sucessfully.
How are you designing the ring of teeth for the pulley? I have the Gearotic software which can create accurate timing pulleys in all sorts of formats. If you need help with that I can send you a PDF for importing into CamBam (that's another plug-in).
Well if you want to get into a new hobby that involves playing with fire, melting aluminium is easy. The YT video below gives you the idea. Use previously cast aluminium alloys (old water pumps from your friendly neighbourhood motor mender etc.) rather than cans or other scrap. Sawing off the bottom of an old fire extinguisher makes a good crucible. Getting a sucessful cast with it is another story however.
Not sure on the use of 2-part plastics for something this robust or how well they machine but one option to consider is to make a master in MDF with your CNC machine and then a silicone mold to cast the final pulley ring, or a blank for final machining. I've done a bit of this for arty stuff but not for engineering. You aren't going to buy from Australia but the Barnes site linked below has info on materials and how to use them. Similar stuff will be available in Pommieland.
https://www.barnes.com.au/
https://www.youtube.com/watch?v=lSoWxG30rb0
Good luck
Kit
I use a free command line dxf generator that can generate all of the main timing pulley profiles, super simple.Quote:
Originally Posted by Kitwn
I just cut an 8m test pulley in 10mm SRBP P1, if came out very nice and extremely strong teeth. I think I will use this material and laminate a few layers together then bolt through, it is pretty cheap stuff and locally available to me.
Attachment 28722 Attachment 28723
That's cheating. Do you have a link for it. :cool:Quote:
Originally Posted by devmonkey
Here you go, https://github.com/paulius-zubaviciu...file-generatorQuote:
Originally Posted by Clive S
You need java to run it.
I made the large timing pulley I was proposing today, it is a 157 tooth HTD 8M (20mm belt) for a project, pulley is ~400mm diameter. It was made from 10mm SBRP with 3 laminations at the rim. Turned out fantastic. I used screwfix cyano to laminate, this makes a very strong joint which you cannot get apart. It will never the less be reinforced with a ring of M5 bolts.
Attachment 28735 Attachment 28736 Attachment 28737 Attachment 28738
What a monster? what's it for may I ask?Quote:
Originally Posted by devmonkey
It is for winching humans into the air attached to paragliders, this pulley forms one side of the winch drum and is driven at around 10kW by a 25kW BLDC motor under FOC control.Quote:
Originally Posted by Voicecoil
Nice! It's very satisfying when the machine you have put so much time and effort into designing and building starts to produce that kind of output.:victorious:
Seconded, that's a lovely piece of work. :cool:
Tool deflection chaps, tool deflection!
So I received a bunch of single flute endmills from China, these things cut aluminium and SRBP nicely. However I'm having some problems, and would like your diagnosis,
So I've just cut a bunch of parts that need a hole that is a reasonable sliding fit on a 25mm shaft. I used one of my new 4mm single flute endmills, 2mm DOC, 1600mm/min into 10mm SRBP. It cuts like butter. However when I measure the hole afterwards it is larger at the top than the bottom by about 0.15mm, effectively the hole is tapered. If I cut the same hole with my usual 6mm 2 flute it is straight.
I assumed this was the single flute deflecting on subsequent deeper passes but it could also be that the endmills are themselves tapered?? What do you think?
I guess the solution is to rough with the single flute and finish with the 2 flute, just a bit of a hassle.
Also could it be that i'm spinning them too fast a 24krpm and they are bowing out due to centrifugal forces?
What happens if you take the feed rate down? And how long is the flute on the single? greater than the depth of the material?
It improves somewhat with slower feed, the flute is longer than the material is deep. I just found one source of the problem the bolts holding the Y axis plate that ties the Z to the Y ballnut were not cranked down, they had worked themselves to just loose, nust have forgotton to loctite those one...
Anyway this tidied up the top diameters which are now spot on again, but with the 4mm bit the hole bottom is still smaller than the top, error is much less, maybe 0.05mm. This is enough to be annoying as you get a decent H8 fit to the shaft on one side and but tight on the other, opening up the hole doesn't solve the problem as it becomes loose on the top. Doesn't matter at all for normal profile work just shaft and bearing fits. I will stick with the 6mm known quality cutters for doing these.
I also just ordered a hopefully decent set of collets from Arc, not convinced by the much cheaper set I have based on the damage they take when you break an endmill.
I've done some more experiments to try and determine the source of the non-vertical walls I get cutting SRBP with single flute endmills. I surfaced the spoil board and trammed the spindle before running these tests.
In all cases the toolpath was a 25mm square in 10mm material, outer roughing profile to 9mm deep leaving 0.2mm for a single finish path at full depth.
#1 4mm Chinese SF, 0.2mm taper top to bottom,
#2 3.175 Chinese SF, 0.1mm taper top to bottom,
#3 6mm Euro SF, 0.03mm taper top to bottom,
#4 6mm Chinese 2Flute, 0.00 taper top to bottom.
The taper is not constant, rather it bulges towards the bottom where the skirt was left to hold the part for the finish pass.
I think that with this slightly flexible material the single flute cutters when slotting are leaving a slot smaller than the tool diameter, this is then cleaned up on the finish pass but not where the tool is cutting the skirt. The same material squeezing does not occur with 2 flute cutters. Has anyone else experience this with single flutes, I haven't noticed this happening in aluminium.
I always find single flutes cut undersize. Never been sure it's a deflection or the tool. I always finish with a 2 flute and I also find HSS gives a better surface finish than carbide in aluminum for the finish passes.
I hardly use Single flute cutters anymore. My preferred method is 3 flute carbide rougher leaving 0.4mm then 1x semi-finish pass @0.3mm and a final 0.1mm final finish pass. For work that doesn't need the best surface finish and accuracy I just take the full 0.4mm as a finish pass.
Quote:
Originally Posted by JAZZCNC
Hi Jazz, what 3 flute rougher do you recommend? I was quite looking forward to making less chips with these 1/8 single flutes but no point if you have to go around with a 6mm 2 flute to clean up,
I mostly cut aluminum and use 8mm reduced neck Alu power cutters from cutwell tools, thou recently I've tried the APT version and they seem ok plus good price.Quote:
Originally Posted by devmonkey
https://www.shop-apt.co.uk/economy-3...-diameter.html
I also tried these and they give a very nice finish, but I've not got enough time on them yet to see how well they last.
https://www.shop-apt.co.uk/3-flute-v...lc-coated.html
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.Quote:
Originally Posted by devmonkey
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.Quote:
Originally Posted by JAZZCNC
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 PicQuote:
Originally Posted by devmonkey
Attachment 28841
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?
Hi
Is it SKU IR26526 profile?
No delete option for duplicate post - sorry:(
HiQuote:
Originally Posted by devmonkey
Is it SKU IR26526 profile?
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.
Attachment 32355
Attachment 32354
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
Attachment 32352
https://www.youtube.com/watch?v=FriMvIZroH4
Result was a perfect grid of blind tapped holes on 50mm pitch, very pleased.
Attachment 32351
Attachment 32353
Attachment 32356
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/Quote:
Originally Posted by devmonkey