Newbie looking at 6040 (China CNC) for polypropylene 15mm sheet

My stock in Fusion is the same size as my actual stock. My part is the same height as the stock so no offsets.

I am manually moving the bit down till it touches the surface. It has been more than accurate for what I am doing. Not 0.3mm out though..

I am pretty sure this is a thing in CAD though not the machine or my physical setup of it.

Quote:

---

Originally Posted by m_c

I wouldn't make assumptions!
Are your previous setups still working as expected?

---

I can test tomorrow.

Are you measuring each piece of stock prior? There can be a lot of deviation on the extrusions, +inaccuracy from the bed and 0.3mm doesn't sound an unrealistic error at all. If you can use stock bottom as part zero and skim the top surface down slightly you will get far more repeatable results.

Also, if milling on a vice, have you trimmed/shimmed it? So that your jaws or soft jaws are square to your axis.

The stock is bang on 15mm.
The 0.3mm is across the length of my part.

I milled my soft jaws while in place so if anything it should be near enough perfect?

Stupidly knocked my soft jaws out of alignment today.

Losing the will to live atm. Looking for quotes for someone else to make them for me.


This machine is okay but I am just unable to get any accuracy when flipping the part, probably down to myself and this shit vice.

Good point about the soft jaws.

Stick at it. Flipping is an acquired art. I would really consider the approach I suggested a few pages back with a fixture plate to use for location and fixing after the flip. It's really quick and easy to make and use and well worth the hour or two it takes to make if you have more than a few parts to make.

No idea where to start in terms of making a fixture plate for these cases...

Vice is easy as I just chop out of the soft jaws the profile of what I am holding.

I have a feeling that this cheap vice is my major problem but also finding the work edge too.
I am now working from the center of my stock/part and using the external sides and halving them to find it, but I am finding it is still off a bit. I think that is more down to the inaccuracy of my probe setup if anything.

All you need for a fixture plate is a method for locating and holding the part and a feature to zero off.

I use dowel pins for locating, all you need is enough space on what will be your bottom surface after the flip for drilling two dowel holes. For fixing I don't think I've ever made anything that doesn't have a spare hole or two to put a bolt through to hold it down, on your cases you could just use stick a bolt through the big square holes with a large washer to grip the sides (one of the clamps that came with the OMIO would do). When you need to do an op on/around one of those bolt holes you just program a pause in your toolpath, move the bolt elsewhere on the part and carry on. For x/y zero I drill and ream a nice round hole to zero off, this is obviously at a known location because you have modeled it in CAD, the same goes for the dowel pins, and therefore from your X and Y zero feature you know where everything is to within the tolerance of your hole and dowel pin sizes, which I've never been off more than 0.2mm across the full 355mm length of the X. Z zero for me is always the top of the fixture plate, then when you're facing down the top of your part you know you are bringing it down to an accurate size.

If that makes sense?

Also another thing, have you checked your x and y axis are square? Because if they're not then you aren't cutting square shapes, you will be cutting trapezoids and that will show up badly with every flip. If you haven't aligned this yourself it will almost certainly be some way out, mine was massively out and took the best part of two days drilling, shimming, and hammering it all into shape.

[edit]

Just milled a part that worked before and it is correct.
Though I added 1mm body that I forgot to add to the setup so it milled 1mm lower in some parts than I wanted it to be.

It milled how the model is set up though so the depth I believe is correct. Will be able to fully check in a min.


I reinstate my comment on it being a Fusion360 thing not the machine or Mach3.

If you think it's fusion, best thing to do is get on the autodesk forum and ask their techs. Their staff are generally quick and helpful at sorting things out, and there are some real fusion brains on there.

No idea what is going on with my Z today. And in general the machine is acting up after working fine for a hour or two.

Just set my Z on my part, ran the program that worked before (doing the same op on the same part to test repeatability) and it just plunged 20mm down into it.
It now thinks the machine cords for Z are 20mm lower than they were just set using 2ref all home".

So I have spent all weekend and this week so far on this problem to no avail.
Had one guy on Fusion forum take a look but he could only simulate it so did not see the problem.

I just noticed on the operation I am running now it looked like it dropped a step.
Wondering if I am taking to much of a DOC or pushing too hard on the feed and it is pulling the bit?
Over time it would result it multiple height differences which I am sort of seeing but some heights are correct.

Once this operation is done ill touch off from the top of my stock and see where it thinks it is.

I have just touched off my part and it is saying it is +1.3mm.
Visually it looks like the bit is further down than it should be so I think it confirms that it is slipping.

I am using the correct collette size and it is tight when I insert the bit.
Not stupid tiht but it grabs onto the bit.
I am not over cranking the thread when putting it onto my spindle as I don't want to over do it. But it is still quite tight.

What is my best option here?

What type of spindle/collet?

If it's ER, then it sounds like you're not tightening it enough. ER collets have to be tight or bits will pull out. There are torque settings for standard ER collet nuts, but typically it's as tight as you can get it with your hands and standard sized spanners, however that's assuming things are well anchored. On a freely spinning spindle, gauging tightness can be a bit tricky.

It's possible to buy replacement ball-bearing collet closer nuts for ER spindles. Arc Euro stock them, as an example. I use these on a couple of different ER collet spindles in my workshop, including the ER20 spindle on my CNC router, and they make tightening the collet much easier.

Quote:

---

Originally Posted by m_c

What type of spindle/collet?

If it's ER, then it sounds like you're not tightening it enough. ER collets have to be tight or bits will pull out. There are torque settings for standard ER collet nuts, but typically it's as tight as you can get it with your hands and standard sized spanners, however that's assuming things are well anchored. On a freely spinning spindle, gauging tightness can be a bit tricky.

---

It is the standard Chinese 2.2Kw one you can grab off ebay for a couple hundred.
ER20.
Ill try it a lot tighter then.

Is there anything I can do to the bit or the ER24 collect light rough it up a bit to get some more grip out of it?

Quote:

---

Originally Posted by Neale

It's possible to buy replacement ball-bearing collet closer nuts for ER spindles. Arc Euro stock them, as an example. I use these on a couple of different ER collet spindles in my workshop, including the ER20 spindle on my CNC router, and they make tightening the collet much easier.

---

Ill take a look, thanks!

Just ran the operation again and I think the same thing has happened again.
Not had a chance to measure yet but it looks like the bit is about 1mm lower than it should be.

Will report back soon


[edit]

Yep, 1.15mm drop on the bit.

Ordered the "ER20 Collet Nut with Ball Bearing - Type A - M25x1.5 Thread", hopefully that is the right one and works...
I also went through all my stock with this problem -_-

Quote:

---

Originally Posted by JOGARA

Just ran the operation again and I think the same thing has happened again.
Not had a chance to measure yet but it looks like the bit is about 1mm lower than it should be.

Will report back soon


[edit]

Yep, 1.15mm drop on the bit.

Ordered the "ER20 Collet Nut with Ball Bearing - Type A - M25x1.5 Thread", hopefully that is the right one and works...
I also went through all my stock with this problem -_-

---

It would be nice if you replied to PMs about the RFQ you posted.

Thanks

Quote:

---

Originally Posted by Chaz

It would be nice if you replied to PMs about the RFQ you posted.

Thanks

---

Thought I replied to everyone. Did I miss you?
If so sorry. Update on the whole thing, we are going to try and machine them here, if it does not work we will continue looking at quotes.

Quote:

---

Originally Posted by JOGARA

Thought I replied to everyone. Did I miss you?
If so sorry. Update on the whole thing, we are going to try and machine them here, if it does not work we will continue looking at quotes.

---

Yep, didnt get any response. No problem.

The STLs you provided were out of scale too, they dont translate to workable CAD parts. They can be converted but Fusion refused. Its better (for future) to export to something other than STL if possible (Step / IGES etc).

Quote:

---

Originally Posted by Chaz

Yep, didnt get any response. No problem.

The STLs you provided were out of scale too, they dont translate to workable CAD parts. They can be converted but Fusion refused. Its better (for future) to export to something other than STL if possible (Step / IGES etc).

---

Yea all the people sending me messages said that.
Though they print fine on my 3D printer exporting that way..??



[edit]
Whats with the off center ring on these collect nuts btw?
I have seen it on both this new ball bearing one and my current one shipped with the machine.

https://s8.postimg.cc/stn4ezcqt/IMG..._123758358.jpg

Quote:

---

[edit]
Whats with the off center ring on these collect nuts btw?
I have seen it on both this new ball bearing one and my current one shipped with the machine.

---

That is to hold the collet in place. You have to wiggle the collet in there. I take it you have been doing this, as this might have been your problem.

Quote:

---

Originally Posted by JOGARA

Yea all the people sending me messages said that.
Though they print fine on my 3D printer exporting that way..??



[edit]
Whats with the off center ring on these collect nuts btw?
I have seen it on both this new ball bearing one and my current one shipped with the machine.

https://s8.postimg.cc/stn4ezcqt/IMG..._123758358.jpg

---

I suspect its the way that our CAD systems are 'interpreting' the STL. I know there are some attributes that you can change when you import but not knowing the 'source', we may not know these and this means that the outputted assumption is wrong.

The fact that I wasnt the only person that said this means that there is something not 100%.

What do you use the make the STL?

Quote:

---

Originally Posted by Clive S

That is to hold the collet in place. You have to wiggle the collet in there. I take it you have been doing this, as this might have been your problem.

---

It's actually to extract the collet from the holder. If you don't clip the collet past the offset lip, then the nut doesn't pull the collet back out when slackened, which can leave you with quite a big headache. Off course not clipping it in also causes uneven clamping, which can lead to excess runout and things not being as secure as they could be...

Quote:

---

Originally Posted by m_c

It's actually to extract the collet from the holder. If you don't clip the collet past the offset lip, then the nut doesn't pull the collet back out when slackened, which can leave you with quite a big headache. Off course not clipping it in also causes uneven clamping, which can lead to excess runout and things not being as secure as they could be...

---

Of course you are correct:redface: My bad.

Quote:

---

Originally Posted by Chaz

I suspect its the way that our CAD systems are 'interpreting' the STL. I know there are some attributes that you can change when you import but not knowing the 'source', we may not know these and this means that the outputted assumption is wrong.

The fact that I wasnt the only person that said this means that there is something not 100%.

What do you use the make the STL?

---

Exporting straight fro Fusion360 by right clicking my part and selecting "save as STL"






But why is it offset?
Wouldn't it also add vibration to the machine?

Quote:

---

Originally Posted by JOGARA

But why is it offset?
Wouldn't it also add vibration to the machine?

---

It's offset so you can get the collet in/out easily.
If it wasn't offset, you'd not be able to get the collet in/out easily, or you risk the collet popping out the nut when trying to remove the nut/cullet from the chuck.

Balanced nuts are available, if balance is an issue.

Trying to reduce the force that is pulling down the bit.

The thing I changed when it started to happen was that I went from 1mm DOC to 1.5mm DOC.
So I am changing that back (sadly the 1.5mm DOC halfs my machine time which is why I want it).

Wondering if the helix is also too much? It sounds nasty when it does it but that could be down to the machine rigidity?

https://s17.postimg.cc/uiuisjc73/Capture.png


I am tempted to grab a 8mm carbide drill bit and use that to get as far down as possible and use that hole as the "pre drill position"

Quote:

---

Originally Posted by JOGARA

Exporting straight fro Fusion360 by right clicking my part and selecting "save as STL"






But why is it offset?
Wouldn't it also add vibration to the machine?

---

Not sure. Perhaps rather saving it as Fusion3D or similar.

Where can I get some oil or whatever to aid with cooling.

Reddit users said my setup for cooling was a bit shit and I have to agree. It is something I have not really looked at improving yet.
They also said my speeds and feeds were wrong for my 6mm roughing bit.

Apparently 12k is wayyyyyy to fast for my feed of 360mm so I am going to try in a bit with 6K and speeding up the feed slowly.

These two things will help resolve my issue.

Quote:

---

Originally Posted by JOGARA

Trying to reduce the force that is pulling down the bit.

The thing I changed when it started to happen was that I went from 1mm DOC to 1.5mm DOC.
So I am changing that back (sadly the 1.5mm DOC halfs my machine time which is why I want it).

Wondering if the helix is also too much? It sounds nasty when it does it but that could be down to the machine rigidity?

https://s17.postimg.cc/uiuisjc73/Capture.png


I am tempted to grab a 8mm carbide drill bit and use that to get as far down as possible and use that hole as the "pre drill position"

---

If you are having these kind of problems now I really dread to think whats coming.

I thought your problem was the cutter being pushed back in the collet not being pulled out? Maybe i need to read back and check that out again. The ramp is fine if anything its to shallow cutters need and want to be worked, sadly you cant do this on a machine like you have. It's just not up to it.

The collet/Nut cutter slippage problem you have. Something is wrong somewhere. These ER systems, although not the best in engineering terms are perfectly adequate for their purpose. Either the collet is out, the spindle taper is out the shank on the cutter tapered. Something is wrong somewhere. It could be you and just lack of knowledge and experience I cant say for definite because i'm not there to see or check whats going on. You are using baby cutters which generate little load and there is no way you need a ball nut for what you are doing. Tightened correctly all should be fine. I cut far in excess of what you are doing by multiple times with ER systems as i have done for years with little issue if ever. It could be a combination of things going on, without someone being there who's knows their stuff its hard to quantify. Also no you should not rough up the cutter or collet or anything for that matter you will solve nothing but will cost your self new equipment when it's buggered up. Plus all this gear is hardened so only serious animalisation would have any effect to 'roughen up'

Regarding your ramp. This is the bottom line, rigidity is everything and more so trying to use helical strategy's because it strains the machine in all directing that traditional tool paths don't. Rigidity is something you do not have, I'm not surprised it sounds bad. In Engineering terms, if it sound bad, it is bad. It's bad for the machine its bad for the cutter particularly and will give premature excessive tool wear so be prepared to be buying many cutters.

You have to work within the restrictions of the machine you have. A machine like that is not capable of very much hence why you can not do very much.

I did also pm you about your RFQ but like Chaz i also had no reply after you sent models that were in a usable format. It was only after mailing you i realised this thread existed which did throw another light on the RFQ and why i had no reply most likely. After seeing this thread it's obvious by first choice you want to try to tackle this job on your own and after buying a machine. No one can blame you for that and i admire anyone that has a go. After reading this whole thread through I do kind of think you went in the wrong direction for what you want to do, the quantities particularly is going to be hard on a time vs money factor unless you have zero value of your time and you physically have the time to be spending so long on each part, plus the times scales you quoted per part are very long indeed. Without proper coolant systems and a tool changer on a machine and one that as the ability to actually cut properly, I think you are really up against it in a big way.

I did offer to give you a run through of your parts on the phone via my pm and explain how you could help yourself a lot with the designs and other details with no obligation on your part. It's pretty much impossible to design parts to be economically manufactured without having a good machine shop grounding. This is what i was offering you FOC with no obligation. I have helped and guided a lot of people on this forum over the years with no obligation on their part. But not replying to people that have spent time looking at this for you is a little off. Their time is also valuable. I'm not annoyed, but it raises peoples eyebrows. I'm just being straight with you.

Without intending to offend anyone who may have advised on this job. I can't go back and read every post to check but things i have noted.

You are using the wrong material. It's expensive by comparison and is not that hard. It cut's fine but it wont help you using tooling plate on this job plus some of it has Anodising problems that you mentioned about some are ok and designed for anodising but you need need to make sure. I don't know why you have chosen tooling plate but you choose the right material for the job not the right material for the machine. The job dictates.

The general process you are using is errrrrrr wrong and long winded. I also have suspicions more is wrong in the background that you have not posted here, especially with the cam side. I appreciate you are restricted by the machine but this again comes down to the time Vs money factor. If you saw your job on a machining center you would wonder why you have been wasting your time and you would see the scale of why you are struggling with this job. 4 tons v what hmm 20 kilos of machine? It's chalk and cheese. Kind of hmm 10 seconds to face a 5 mm cut of a, ally block 3 inches wide and 4 long if that, as a simple and crude example. The difference is, you tell the machine what to do with the part as where your machine is telling you what you can do to the part.

Sorry it's long winded but its observation of the is entire thread being as i have not posted in it so far.

I hope you can at least find a few things that are helpful and sheds a bit of light on things for you.

All the best

Quote:

---

Originally Posted by spluppit

If you are having these kind of problems now I really dread to think whats coming.

I thought your problem was the cutter being pushed back in the collet not being pulled out? Maybe i need to read back and check that out again. The ramp is fine if anything its to shallow cutters need and want to be worked, sadly you cant do this on a machine like you have. It's just not up to it.

The collet/Nut cutter slippage problem you have. Something is wrong somewhere. These ER systems, although not the best in engineering terms are perfectly adequate for their purpose. Either the collet is out, the spindle taper is out the shank on the cutter tapered. Something is wrong somewhere. It could be you and just lack of knowledge and experience I cant say for definite because i'm not there to see or check whats going on. You are using baby cutters which generate little load and there is no way you need a ball nut for what you are doing. Tightened correctly all should be fine. I cut far in excess of what you are doing by multiple times with ER systems as i have done for years with little issue if ever. It could be a combination of things going on, without someone being there who's knows their stuff its hard to quantify. Also no you should not rough up the cutter or collet or anything for that matter you will solve nothing but will cost your self new equipment when it's buggered up. Plus all this gear is hardened so only serious animalisation would have any effect to 'roughen up'

Regarding your ramp. This is the bottom line, rigidity is everything and more so trying to use helical strategy's because it strains the machine in all directing that traditional tool paths don't. Rigidity is something you do not have, I'm not surprised it sounds bad. In Engineering terms, if it sound bad, it is bad. It's bad for the machine its bad for the cutter particularly and will give premature excessive tool wear so be prepared to be buying many cutters.

You have to work within the restrictions of the machine you have. A machine like that is not capable of very much hence why you can not do very much.

I did also pm you about your RFQ but like Chaz i also had no reply after you sent models that were in a usable format. It was only after mailing you i realised this thread existed which did throw another light on the RFQ and why i had no reply most likely. After seeing this thread it's obvious by first choice you want to try to tackle this job on your own and after buying a machine. No one can blame you for that and i admire anyone that has a go. After reading this whole thread through I do kind of think you went in the wrong direction for what you want to do, the quantities particularly is going to be hard on a time vs money factor unless you have zero value of your time and you physically have the time to be spending so long on each part, plus the times scales you quoted per part are very long indeed. Without proper coolant systems and a tool changer on a machine and one that as the ability to actually cut properly, I think you are really up against it in a big way.

I did offer to give you a run through of your parts on the phone via my pm and explain how you could help yourself a lot with the designs and other details with no obligation on your part. It's pretty much impossible to design parts to be economically manufactured without having a good machine shop grounding. This is what i was offering you FOC with no obligation. I have helped and guided a lot of people on this forum over the years with no obligation on their part. But not replying to people that have spent time looking at this for you is a little off. Their time is also valuable. I'm not annoyed, but it raises peoples eyebrows. I'm just being straight with you.

Without intending to offend anyone who may have advised on this job. I can't go back and read every post to check but things i have noted.

You are using the wrong material. It's expensive by comparison and is not that hard. It cut's fine but it wont help you using tooling plate on this job plus some of it has Anodising problems that you mentioned about some are ok and designed for anodising but you need need to make sure. I don't know why you have chosen tooling plate but you choose the right material for the job not the right material for the machine. The job dictates.

The general process you are using is errrrrrr wrong and long winded. I also have suspicions more is wrong in the background that you have not posted here, especially with the cam side. I appreciate you are restricted by the machine but this again comes down to the time Vs money factor. If you saw your job on a machining center you would wonder why you have been wasting your time and you would see the scale of why you are struggling with this job. 4 tons v what hmm 20 kilos of machine? It's chalk and cheese. Kind of hmm 10 seconds to face a 5 mm cut of a, ally block 3 inches wide and 4 long if that, as a simple and crude example. The difference is, you tell the machine what to do with the part as where your machine is telling you what you can do to the part.

Sorry it's long winded but its observation of the is entire thread being as i have not posted in it so far.

I hope you can at least find a few things that are helpful and sheds a bit of light on things for you.

All the best

---

Hi Spluppit

Thanks for the reply and sorry for not replying to your quote. I thought I got back to everyone but must have missed out on a few.
To be honest it has been a bad couple weeks, I am a few months behind on this project, moving house next week and my dog has been ill. So this has all been stressing me out.

The bit is being pulled out. Resulting it it cutting too much on the Z axis. My 12mm depth is resulting in 12.6-13mm
Should I try and increase the ramp speed a bit and see if that improves things? I think I am taking everything too general which has resulted in poor performance. That being said, some of the parts I have had out of it have been great.

Predrilling a hole for each case is my best bet then for the rigidity problem?

Again sorry for not replying. Just not running on all cylinders the past couple weeks.

I picked the eco cast on recommendation of it being simple and easy to cut on the machine as well as having decent surfaces that I could use for product surface finish. I have not had a problem with the anodising. Other than my fuckup eary on the EcoCast has taken anodising well. What should I be using on this machine?

I understand a proper machine will joblot all 160 cases in a day or two but I didn't have the money for it.
I was quoted before I joined here around £60 per case. I felt that I could buy a machine and learn enough to make them. It is why I designed the case to be really simple though obviously it has not been as smooth and as fast as I would have liked.

Overall the parts I have had from the machine have been fine. It is just this last issue really that is holding us back.
https://s17.postimg.cc/4hp400lb3/IM...201123_HDR.jpg
https://s17.postimg.cc/f4ix5fe0v/IM...936926_HDR.jpg

I have been advised to lower my RPM and improve the coolant so tomorrow I will get a chance to try that out and see if that fixes the problem.
If not, idk.

Thanks for all the info, I understand it is hard to work out what is wrong when you are not in front of the machine and having some idiot on the other side trying to explain what is going on.

Jack,

For coolant, unless you can get good flood coolant, the next best option is air with a bit lubricant.

The key thing with nearly all machining, is to get chips away from the cutter. Getting chips away is even more critical with aluminium, as it can be very prone to chips welding to the cutter, which is never good and often fatal for the part, cutter of both.

I managed for a good few months machining aluminium with just WD40 and compressed air. I'd set the machine running, spray a bit WD40 on, hit cycle start, then wander back every couple minutes and blow chips of the part, and a little bit extra WD40 if it looked like things were getting too dry. I only used enough WD40 to give a light coating on the part/cutter to help stop chips sticking. If I knew there was a critical cut coming up I.e. spiral in, or deep slot, I'd stay and hold the air on the cutter to ensure no chips built up, and add in a bit extra WD40.
The WD40 does make the chips clump together more and a bit harder to blow away, but the trade off was they were less likely to weld to things.

I eventually made a mister, which removed the need for as much babysitting, but it would still need a bit extra assistance in deeper parts.

Quote:

---

Originally Posted by JOGARA

Hi Spluppit

Thanks for the reply and sorry for not replying to your quote. I thought I got back to everyone but must have missed out on a few.
To be honest it has been a bad couple weeks, I am a few months behind on this project, moving house next week and my dog has been ill. So this has all been stressing me out.

The bit is being pulled out. Resulting it it cutting too much on the Z axis. My 12mm depth is resulting in 12.6-13mm
Should I try and increase the ramp speed a bit and see if that improves things? I think I am taking everything too general which has resulted in poor performance. That being said, some of the parts I have had out of it have been great.

Predrilling a hole for each case is my best bet then for the rigidity problem?

Again sorry for not replying. Just not running on all cylinders the past couple weeks.

I picked the eco cast on recommendation of it being simple and easy to cut on the machine as well as having decent surfaces that I could use for product surface finish. I have not had a problem with the anodising. Other than my fuckup eary on the EcoCast has taken anodising well. What should I be using on this machine?

I understand a proper machine will joblot all 160 cases in a day or two but I didn't have the money for it.
I was quoted before I joined here around £60 per case. I felt that I could buy a machine and learn enough to make them. It is why I designed the case to be really simple though obviously it has not been as smooth and as fast as I would have liked.

Overall the parts I have had from the machine have been fine. It is just this last issue really that is holding us back.
https://s17.postimg.cc/4hp400lb3/IM...201123_HDR.jpg
https://s17.postimg.cc/f4ix5fe0v/IM...936926_HDR.jpg

I have been advised to lower my RPM and improve the coolant so tomorrow I will get a chance to try that out and see if that fixes the problem.
If not, idk.

Thanks for all the info, I understand it is hard to work out what is wrong when you are not in front of the machine and having some idiot on the other side trying to explain what is going on.

Jack,

---

Please also send me the fixed files (ie Step or Iges from Fusion or the raw F3D) so that I can look at how long it will take the machine these. Can give my 2p worth as well. Free to use / not use the info.

Quote:

---

Originally Posted by m_c

For coolant, unless you can get good flood coolant, the next best option is air with a bit lubricant.

The key thing with nearly all machining, is to get chips away from the cutter. Getting chips away is even more critical with aluminium, as it can be very prone to chips welding to the cutter, which is never good and often fatal for the part, cutter of both.

I managed for a good few months machining aluminium with just WD40 and compressed air. I'd set the machine running, spray a bit WD40 on, hit cycle start, then wander back every couple minutes and blow chips of the part, and a little bit extra WD40 if it looked like things were getting too dry. I only used enough WD40 to give a light coating on the part/cutter to help stop chips sticking. If I knew there was a critical cut coming up I.e. spiral in, or deep slot, I'd stay and hold the air on the cutter to ensure no chips built up, and add in a bit extra WD40.
The WD40 does make the chips clump together more and a bit harder to blow away, but the trade off was they were less likely to weld to things.

I eventually made a mister, which removed the need for as much babysitting, but it would still need a bit extra assistance in deeper parts.

---

My current system is one of those cheap bendy hoses with air and "mist".
I have pretty decent air going through it with a tiny amount of regular water and have not had any chip welds.

Probably could do with some sort of coolant fluid or additive in the water though to assist.

Quote:

---

Originally Posted by Chaz

Please also send me the fixed files (ie Step or Iges from Fusion or the raw F3D) so that I can look at how long it will take the machine these. Can give my 2p worth as well. Free to use / not use the info.

---

Ill leave this public for now, will take down at a later date http://a360.co/2zPSUYP

Thanks

Quote:

---

Originally Posted by JOGARA

My current system is one of those cheap bendy hoses with air and "mist".
I have pretty decent air going through it with a tiny amount of regular water and have not had any chip welds.

Probably could do with some sort of coolant fluid or additive in the water though to assist.

---

Is the air flow enough to blow the chips well out the way?
Provided it's keeping chips well away from the cutter, then your setup should be fine. Even if you have to give an extra blast occasionally, it sounds like you've got a reasonable setup, and I wouldn't worry.

It might be worth trying some of the misting fluids though. This is what I used to use - http://www.johnnealeltd.co.uk/shopenvirocutse10.html

Quote:

---

Originally Posted by m_c

Is the air flow enough to blow the chips well out the way?
Provided it's keeping chips well away from the cutter, then your setup should be fine. Even if you have to give an extra blast occasionally, it sounds like you've got a reasonable setup, and I wouldn't worry.

It might be worth trying some of the misting fluids though. This is what I used to use - http://www.johnnealeltd.co.uk/shopenvirocutse10.html

---

Yea the chips fly miles. I found tiny amounts of water and decent air meant that 99% of the chips left my stock area.
The ones left tend to stick along the walls of my part. Not a massive problem as I then go around with my finishing path and I do that dry (only taking off 0.25mm) and that clears whatever is left from me brushing away the majority of leftovers.

That Envirocut SE10 looks good. I like that it is biodegradable. I am using a tiny amount of coolant as it is so 1L should do me for a while?

Just tested the machine with 1mm DOC at 6000 RPM and it was fine.
Pushed the machine with a face operation of 100% WOC and only when at 720mm feed it made a bit of noise.

So going to try it on part. Obviously not 100% width.

Will quickly try a couple helix with the new speed and faster plunge.

Just ran the operation and it thinks the top of the stock is +1.7mm

No idea what to do...

Contacted Omiocnc so lets see what they think.

Re: Finishing and part quality.

First of all please do not think i am purposely going out of my way to make you feel bad or I'm being difficult. You have come a long way since the beginning of your post to actually making parts from knowing very little. You should be proud of that and well done. I have tried to gently explain you are a world away still. It really is not as simple as people think at times as buying a machine and making parts. I did a 5 year Toolmaking apprenticeship and 4 years at college and before that i was still on the shop floor for a year before they were satisfied to put me through the apprenticeship etc. Then you are still not considered accomplished that takes another 5 to 10 years. On top of that i have always been in machine shops and workshops since i was a child and had a natural aptitude for the Job. I hope you can try to see this as more a education rather than criticism.

I do not agree that your parts are fine. Without seeing any images of your finished parts, I said you were using the wrong material and the evidence is those images you posted. I appreciate images can be a little deceiving online but i have seen and taken enough to hopefully know what im looking at. Yes your parts are anodised but that is a very broad use of the term, in the fact they have been dumped in a sulfuric tank with some current and then dyed. But that's as far as it goes. The finish is flat and and one one those images shows very blotchy uneven finish and a lot of surface marks. Cosmetics is as important as the function of the item in today's word if its a product people will see and use. (more so if they are paying decent money for it) I did read about you tumbling or vibratory finishing these parts. There are a ton of variables with finishing which i cant go into here but I feel its the wrong move if you understand the anodising process. (Don't slate me for saying this guys, as i said i cant go into full detail) A quick debur if necessary fine but.. the rest hmmmm. By rights parts like this you anodise off the machine. This is 2017.

Also finding a good anodiser is very hard indeed. I know from loosing thousands of pound to idiot ones out there in past years. With this in mind there could be an element of error from the anodiser as i said good ones are very hard to find. I cant tell categorically because I'm not there to see in the flesh. If your anodiser has not mentioned about the quality of the finish on the part or his anodising don't use him is my advice.

You have taken the path of least resistance (on advice granted) to get to your end goal, sadly it does not work like that in manufacturing. I mean this is the politest way but i get the feeling some of the problems is you don't actually know what you are looking at yourself to decide if its acceptable or not.

The result of the part is only as good as the work gone into it.

These images taken last night are literally bits laying about the workshop and these are scrap for various reasons, finishing being one of them. A lot of these parts are very old indeed most of the anodised parts are anything from a year old to up to 25 years old or so. The bare Aluminum parts are straight off the machine, you can anodise straight off this, no finishing and you will get a beautiful satin jet black uniform finish, of course requiring an anodiser who is not a banana eating Orangutan. I could not find a lot of black anodising laying about, but there are few bits and i'm sure you can see the difference.

I will reply to your other post to me in more detail when i get a chance. Also to mention about the cost you were given of £60.00. If you read my pm you will see i explained that you are making the part expensive, the models are not compete for a start, plus you have now altered one. I said about having a chat on the phone to reduce this cost because i expect typically, the tight rads that are probably not necessary plus many other things that can help. This is why you got a very inflated quote. They looked at the part and glazed over, exactly as i did but i offered help, to help you reduce the cost. They should be no where near the price you have been quoted with a little work to make it easier on the manufacturing. You would pick the parts up tapped holes as well.

Its a package deal, knowing how to machine to design economically to machine economically. You cant learn that in 10 months or so.


Attachment 23287Attachment 23288Attachment 23289Attachment 23290Attachment 23291