Frage Problem with dimensions, using fusion 360 uccnc

Hi guys, hopefully I've posted in the right section. I have run into a strange problem in that I am getting incorrect dimensions after milling. I've added a couple of pictures to show. the boxes should be 50mm outer width and 40mm leaving a 5mm pocketed area and clearly they are not. The circle and ring should be 10mm and 15mm diameter but they are 14mm and 21mm. Pocketed area on the ring should be 5mm, it's about 3mm. Depth is also out, the ring should be 2mm deep but it is 3mm. The circle should be 4mm but is 6mm. The strange thing is I also did a contour cut with tabs (not pictured) and the tab height is actually correct. The other strange thing is I had recently changed back to windows 7 and reinstalled all associated software but before this I had no problem with dimensions. The problem is consistent though as I cut 4 rectangle pieces and they are all exactly the same, wrong size as per drawing but no discrepancy between them. The alloy ring pictured was cut prior to the reinstall and is accurate per drawing. I noticed the Z dimension when cutting was correct, which could indicate a tool length error input from me but the fact that I was using the same tool from the library from previous successful cuts rules this out. I have absolutely no idea what is going on nor where to start to fix. Any help is greatly appreciated.

Ok problem sorted, after running the calibration as suggested by cncdrive the issue was with the steps and it was at 200 and it should be 133.33. After digging deeper it seems the earlier version 1 stepcraft machines were at 200 steps and I suspect my stepcraft profile for uccnc was for the older version and when I was given a replacement stepcraft profile from cncdrive it was for the older stepcraft v1 machines.

Hi,

Interested to see you have milled an aluminium part successfully. I had a disaster on my first attempt and broke the cutter when everything jammed up.

I haven't tried since, but would greatly appreciate information on the grade of Al you used and cutter details (size, spindle speed, feed and plunge speeds etc).

Regards

Peter

peterg1000 schrieb: Hi,

Interested to see you have milled an aluminium part successfully. I had a disaster on my first attempt and broke the cutter when everything jammed up.

I haven't tried since, but would greatly appreciate information on the grade of Al you used and cutter details (size, spindle speed, feed and plunge speeds etc).

Regards

Peter

Hi Peter, sure I can tell you what I did, and I can tell you now it wasn't all good with my first cuts too , in fact they were horrible (see pic) and I also went through some cutters. The alloy was 6061. Cutting feed rate was 1000mm/min, plunge was at 10mm/min, spindle speed was at its lowest which I believe is 10,000 rpm, its a kress 800 spindle motor. I took multiple cut depths at .1mm, I did try .2mm and it seemed fine but I just felt more comfortable at .1mm, I will likely try more at .2mm again. Also I ramped in, I'm still very new to this so I'm not sure if lead in will give same results as ramp but I'm assuming it would be similar. Cutter was 2 flute 2mm carbide. I used air blast and wd40 for lubrication. I'm concerned about tool life but until I can cut some more I just don't know life expectancy from these cutters. Also included another pic of some test cuts with depth cuts at .1mm and .2mm.

Hi Sc420user,

Much appreciate your feedback on aluminium cutting - gives me a proven starting point for another attempt. Interesting that you used a relatively low spindle rpm and a high feed rate as well as lubrication and chip clearance.

I would guess that your carbide cutters would last pretty well from the wear point if view as long as they don't break in the meantime!!

Regards,

Peter

Happy to share. Yes I had tried varying spindle speeds and low feed rate of about 130mm/min to 200mm/min but as you can see by the first picture it was basically a disaster. I asked about it over on cnczone and was suggested to try a much higher feed rate, although skeptical at first the results speak for themselves. I am keen to cut some more but as I have only just built the machine about 6 months ago and now more experienced, I have noticed a possible alignment issue where it is machining a little out. So I need to deal with that first. Anyway good luck with your next attempt at the alloy and hope you have some success.

I had a go at cutting 3/64" (1.2 mm) aluminium sheet (grade unknown) this morning. This piece is a foldable net for a frame to hold six DPDT parallel slide switches. The test cut in plywood illustrates the shape.

It is a 2.5D cut which consists of 17 mounting holes 2.5 to 2.7 mm diameter, six apertures and an outline.

Feed rate: 1,800 mm/min
Plunge rate: 30 mm/min (normal, not ramped or helical)
Spindle speed: 20,000 rpm
Cutter: 2 flute, 2 mm solide carbide TiAlN coated, 5 mm flute length.
0.2 mm depth per pass, six passes for each shape.

As you can see it was not successful but it wasn't a complete failure either. I gave up on the holes after the third one when I could see the swarf melting and moved on to the outline cut using a separate toolpath. Thankfully the sideways full depth plough after the machine lost steps did not break the cutter. It seemed o.k. up to the third pass.

I used MeshCAM to generate toolpaths then extracted the G Code for the pencil cleanup finishing passes then compiled the final file manually.

The big problem here is that the swarf melted and piled up around the channel.

My next attempt will be with a lower feed rate for sure and possibly a lower spindle speed too. I am looking at getting a portable 240 V air compressor for cooling too.

Doug

Doug I had the same problem with some 5005 alloy,I think it is because of the softer alloy. I would definitely use an air blast of some sort to keep cutter cool as heat will kill your cutter. I haven't tried any other settings with that alloy because I don't intend to use it. I would do as you say and slow your spindle and feed down. I am currently cutting 6061 at 900mm/min, spindle at circa 12500 rpm and DOC at .3mm

Thanks! I think 900 mm/min, spindle speed 12500 rpm will work better

I'm not sure that sheet is available in the harder alloy grade but I'll check it out.

Doug

See attached finished, switch frame net which has taken most of the day to produce.

This was cut at 0.1 mm depth per pass at 900 mm/min feed and 12,500 rpm. No cooling but I stopped after every switch aperture. I scored the drill holes with one 0.1 mm pass just to mark the position then drilled them manually. The outline was run on 12 continuous passes. No lost steps although there was a lot of vibration.

Today's result was only slightly better than the previous attempt and is not an exercise I want to repeat any time soon! No video because it was not a pretty sight!

Basically, I have had to hand finish it over several hours because the cut was a mess. The only positive out of this is that it looks more like Brian May's original hand made item!

I would now conclude that the grade of aluminium is the key factor here. This eBay sheet is horrible. Rory recommends 6082T6 and is quite adamant that it can bd successfully milled at higher feed rates and spindle speed but harder grades are difficult to find in small thicknesses.

Doug

Hi Doug, certainly in Australia it is also hard to find harder grade alloys in thin sheet. I have cut some supposed 7075 from china bought on ebay and it cut quite well with the above feed rates, although skeptical at first buying from china it may very well be 7075.

Here is an item number of some sheet off the same seller I bought from. You could also search for 7075.
171860413907

Here is some 6060 I cut over the weekend. I had a problem with z axis coming loose and broke 2 cutters before I realised, I think the cut would have been much better had the axis not been loose although it came out acceptable but not really what I wanted. I have some new single flute cutters I will be trying too.

Hi Doug,

6082 T6 is available in UK, check Ebay, I have purchased sheets of different thickness's starting at 1.5 mm going upwards.
The normal aluminium available 'off the shelf' is very often pure aluminium which is soft.
You may find reference to a 6061 aluminium type (mainly available in USA) which is good for us to use, 6082 is a very close alternative more readily available in Europe.

Not able to gve any figures for cutting as not yet used it.

alan

Hi guys.

Thanks for the tips. I saw 1.5 mm 6086T6 sheet on eBay. Unfortunately that is too thick for my precise requirements. 1.0 or 1.2 mm is what I need. This supplier looks plausible if I'm reading their website correctly:

www.ssaltd.net/index.php/aluminium-stock/aluminium-grade-6082

I suppose there is the option of milling 0.3 mm off the stock in the cutting region on the 1.5 mm sheet with a larger diameter cutter but that is rather too much work. This is a piece which can be made in a day or two by hand by drilling bits out so I have to weigh up the time, cost and trouble of using CNC against the manual labour involved. I only need one piece now but if I decide to make them for other replicas in future, I would like to finalise a toolpath and material supply chain at this stage.

I'll check out the 7075 grade suggested too and keep looking. Aluminium Droitwich sells a lot of aluminium sheet, rod and bar on U.K. eBay. Perhaps I'll send them a message and ask if they can supply a harder grade sheet suitable for milling in 1.0 or 1.2 mm thickness to special order.

Regards.

Doug

Ive cut 1050 aluminium with success which is very soft with 99% purity.
You could try 5251 which you can buy in the thickness you require.
Try a single flute endmill and make sure the material is held down well if its a thin thickness.
Use some lubricant. I find cutting 6082 the best to cut with a beautiful milling finish.

Thanks for all the tips guys.

Looking at data sheets for the various grades mentioned, there is usually a qualitative "machinability" quoted but I guess the quantitative Brinell Hardness factor is what best relates to how well the grade will machine.

I sourced 1050 H14 for my original cut. H14 refers to the temper which is quoted as "Work hardened by rolling to half hard, not annealed after rolling." Machinability is "poor" and Brinell Hardness is 34 HB.

I have just bought some sheet which is an equivalent grade to 5251 H22 (300 x 300 x 1.2 mm thickness) from Merlin Motorsport in the U.K. Temper is "Work hardened by rolling then annealed to quarter hard", machinability is "average" and Brinell Hardness is 56 HB. I will attempt the cut again with some compressed air cooling to see if this harder grade yields a better result.

6082 T6 grade is recommended to be one of the most suitable for machining. Temper is "Solution heat treated and artificially aged", machinability is "good" and Brinell Hardness is 89-91 HB depending on plate thickness. A value is not quoted for sheet/plate below 6.0 mm thickness on the Aalco Metals datasheet.

Regards.

Doug

Hi,

the Alloy AlMg4.5Mn0.7 should be very good for milling.
This is ISO 5083 grade.