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

Zeeflyboy, any suggestions on where to start with the TPA-2?

Not been given any docs other than this;
http://kurokesu.com/main/2015/12/30/...robe-to-mach3/

I'm afraid I don't use the same motion controller as you, nor do I use Mach3 anymore... but it should be fairly straight forwards.

Hook it up to the same point that the normal probe goes to, but you just need to go to the ports and pins part to invert the signal mach is looking for as it's a normally closed circuit vs normally open. If you flip over to the diagnostics page of mach you should then be able to see the probe input trigger as you press on the probe tip.

It is definitely worth spending a couple of minutes dialing in the probe tip using a dial indicator before each use - the runout of the spindle/collets results in me getting anything up to around 0.1mm of runout all the way down at the tip which will affect any probing results. Within a couple of minutes of careful tweaking I can get that down to less than 0.01mm

As for probing on mach3 - I've never done it. I think there were some screen sets for mach3 that have probing built in, or you could write a small macro to do it (or use someone else's) but the info is out there if you have a look. Mach4 makes things quite simple with a dedicated probing section built in so I've never had to figure anything out in that regard.

Quote:

---

Originally Posted by Zeeflyboy

I'm afraid I don't use the same motion controller as you, nor do I use Mach3 anymore... but it should be fairly straight forwards.

Hook it up to the same point that the normal probe goes to, but you just need to go to the ports and pins part to invert the signal mach is looking for as it's a normally closed circuit vs normally open. If you flip over to the diagnostics page of mach you should then be able to see the probe input trigger as you press on the probe tip.

It is definitely worth spending a couple of minutes dialing in the probe tip using a dial indicator before each use - the runout of the spindle/collets results in me getting anything up to around 0.1mm of runout all the way down at the tip which will affect any probing results. Within a couple of minutes of careful tweaking I can get that down to less than 0.01mm

As for probing on mach3 - I've never done it. I think there were some screen sets for mach3 that have probing built in, or you could write a small macro to do it (or use someone else's) but the info is out there if you have a look. Mach4 makes things quite simple with a dedicated probing section built in so I've never had to figure anything out in that regard.

---

Thanks for the info. The probe does look a tad off from stock. I forgot to get a dial indicator >.<

Trying out the ProbeIt plugin that creates a wizard to probe. It has tools like auto calibrate. Uses a known diameter though and I don't know if I got anything for that :/
Trying to think what I can get that is large enough but not going to break the bank...

in reality you probably don't need to calibrate it.... if probing the inside of a hole for example, everything is relative so you will still find centre of the hole even if the measured dimensions were off.

Calibration is more of interest if you were measuring things for verification purposes.

0.03mm is the best I have gotten so far.
Finding it quite hard to get it any closer :/

https://media.giphy.com/media/3o7aCY...gWCQ/giphy.gif


Is there a way to get Mach3 to move a single step? 0.01mm is a couple steps on the stepper from the looks of it.
And how accurate is the mm readout in the interface? I would rather it move to the nearest 0.01mm rather than this...

https://s1.postimg.cc/98ypvmenqn/Capture.png

Typical stepper is 200 steps per revolution. You have 5mm screws, so you move 0.025 per step (5/200).

Microstepping doesn’t really count, so the fact you have eg 320 per unit (can’t remember exactly what the stock setup is) isn’t really what you’re looking at, though you could argue with little to no load it won’t be far off.

That said, I can move mine in 0.01mm steps on the jogging button but I have 1.2 degree steppers (so 0.017mm per full step) with built in encoders and microstepping gives 800 per unit.

Just edit your jog values so that one of them is 0.01mm and it’ll do it’s best to match. If it is 320/unit then you have a base value of 0.003125 so any movement will be a multiple of that - that means the closest movement to 0.01mm you could theoretically get is 0.009375 which is why the value in the readout looks a bit odd - it’s physically impossible for it to move to any value that isn’t a multiple of 0.003125. Again though microstepping is not really reliable regarding accuracy so your “real” resolution is 0.025 as limited by the motor steps per degree and the pitch of the ball screw.

Btw I would try to use the least amount of travel on the dial indicator - those type can have a fair bit of spring push and you may be deflecting the probe rod slightly. No guarantee that the deflection is equal all the way around.

Do you actually need to jog into the dial for this? I just spin the guage zero so that it sits in the middle of the values for either side and then adjust probe until it reaches close to zero, then move to the next set of screws and repeat, then go back to the first as it may have moved slightly. That will normally get runout to less than 0.01mm for me. Definitely a bit of a knack to it but it only takes me a few minutes now.

Oh and finally have you tried calibrating the machine? Mine wasn’t exactly wonderfully accurate out of the box. I think mach3 even has a screw calibration wizard that saves you doing the maths.

I have not changed anything other than adding ProbeIt to the wizard.
Don't like messing with stuff.

This is default.
https://s1.postimg.cc/79q0xvnwsv/Capture.png

What would be the highest resolution I can get from this without it being too weak?
That and roundest number possible :p


I moved back on the indicator and got around 0.025mm so tiny bit of movement yes.



Ideally I want to be able to probe my soft jaws and just batch process a load of cases.
Changing tools all the time takes time.

The only way around this is to mill the outside and front of my case first, then flip and mill inside with the degree of error being around 0.05-0.075mm.
This would allow me to vacuum plate the first operation on the front of the case, removing the need for super glue.

I think I could live with that...

Ideally I could get it all bang on but that is not looking like it is going to happen on this machine any time soon... :/

I wouldn't get overly obsessed with the DRO giving a round number read out - better that it is actually calibrated correctly.

After all, other than for reasons of OCD consider that your 17.9188 from the DRO above is only 0.0012mm away from the commanded 17.92 - 0.0012mm is roughly half the width of a typical bacterium (which are commonly 0.01mm long too for context!) Basically it's a level of precision that your machine couldn't possibly hope to achieve anywhere near so it's irrelevant for all but how neat the DRO looks.

When you correctly calibrate the ballscrews, likelihood is that you will end up with a horrendous number like 321.24 as your calibrated steps per mm which of course means you don't have a snowball's chance in hell of ending up at a round number on the DRO.

I'm not sure how you arrive at your conclusion that you will be working to an error of 0.05 to 0.075mm.... but 0.05mm is nothing to be sniffed at... it's a very good level of accuracy realistically speaking - less than the thickness of a typical human hair.

Increasing the microstepping won't really help... if anything it just makes it harder for your motion controller to keep up at high speeds. Microstepping really only serves to make things smoother, gains in resolution are mostly illusionary.

Sorry I meant 0.5-0.75mm.
I think it will be fine. Just need to rework a few things in my CAM

Thanks for the info

I have the same machine. A couple of things. I have recently done a batch run like what you're wanting to do. I did it by marking my vice with a bit of white electrical tape and eyeballing the edge of the stock up to it, drilled all the holes with the same drill bit (smallest hole size, the larger holes I opened it manually with a cordless whilst the next part was on the machine) on the vice then moved them over to a fixture plate for profiling, located by two dowels after reaming two of the holes by hand, then ran the profile paths, chamfer, flip, chamfer.

If you are touching the home switches at any point, don't. They are lousy and will introduce anywhere between 0.04 to 0.32 error on each axis. The machine itself isn't so awfully bad at repeatability, there is a bit of backlash in mine but it ran the ops on all 6 of the parts I made without any major visual error. I chucked up my dti between each tool change and rezeroed off the reamed hole on my bed I use as a reference just to be sure but it was probably a waste of time.

To step jog, press tab on your keyboard in mach3 and you can change between continuous jog mode and step jog, and also change the step value. Spinning a dti in a reamed hole to find zero I use 0.01mm step and I'm normally back out the hole and putting a tool in within a minute.

Tool changing is the enemy. My z setter is nuts for some reason and will never give close to the same result twice so I've been z setting with a feeler gauge for awhile, takes a little longer but it's absolutely on point. Cleaning the spindle taper, spindle threads and collet nut between each tool change is also a real bastard (I've just ordered a second collet nut so I have one clean with the tool mounted ready to screw in). And also spend far too much time making sure I have the mist nozzles pointing in the right place.

Well you should certainly be able to do a lot better than that... why do you think you'll be stuck with that level of inaccuracy?

My admittedly limited testing has showed the probe (runout adjusted each time) to find centre of a bore to within less than 0.02mm.... a quick way to check this is to run a centre probe, take a note of the Machine co-ordinates rather than the work co-ordinates, clock the probe eg 90 degrees and run the centre probing again. note how much the machine co-orindates have changed by after it re-zeros, repeat that a few times at different clocks and the maximum variation in machine co-orindates gives you a good indication of how reliably it is finding centre.

Finding zero from probing two edges to find a corner is a slightly different kettle of fish as you would need to calibrate to take account of deflection before the probe triggers to get truly accurate results. Centre probing mostly gets rid of this issue as deflection occurs on both sides.

If machining using a jig/soft jaws, you can always ream a bore in the jig/jaw that will then serve as your zero point.

I would say with a bit of thought you should certainly be able to get two sided machining to within a very tight tolerance (in terms of repeatability - absolute accuracy is another question as you could for example be eg 0.1mm out on all dimensions but as they will all be the same then relative to each other it doesn't matter).

Quote:

---

Originally Posted by Snapper

Tool changing is the enemy. My z setter is nuts for some reason and will never give close to the same result twice so I've been z setting with a feeler gauge for awhile, takes a little longer but it's absolutely on point. Cleaning the spindle taper, spindle threads and collet nut between each tool change is also a real bastard

---

I do something very similar these days - I have a reel of 0.01mm shim steel and I jog the tool up to just short of the z-zero surface, then jog in 0.01mm increments while sliding the shim material back and forth. Once it grabs you know you are 0.01mm above the surface and it works rather well for me.

Interesting point about cleaning between changes... Until relatively recently I never paid much heed to this and the amount of gunk that I managed to clean out of my spindle bore was eye opening. more than halved my runout by cleaning it out.... now every tool change I use compressed air to clean out the collets and bore, and usually a piece of oiled kitchen towel to wipe out the bore before then re-inserting the new collet if changing collet size.

Quote:

---

Originally Posted by Zeeflyboy

I do something very similar these days - I have a reel of 0.01mm shim steel and I jog the tool up to just short of the z-zero surface, then jog in 0.01mm increments while sliding the shim material back and forth. Once it grabs you know you are 0.01mm above the surface and it works rather well for me.

Interesting point about cleaning between changes... Until relatively recently I never paid much heed to this and the amount of gunk that I managed to clean out of my spindle bore was eye opening. more than halved my runout by cleaning it out.... now every tool change I use compressed air to clean out the collets and bore, and usually a piece of oiled kitchen towel to wipe out the bore before then re-inserting the new collet if changing collet size.

---

I use a thicker 0.55mm gauge purely because it's more solid so easier to keep straight and flat. I eyeball down then step jog back up until it fits under.

Yeah cleaning everything is absolutely paramount to getting a nice cut. Specially with alu, chips get in the slots in the collet and cause absolute carnage. I use isopropyl alocohol on paper towel. It's quite amazing just how much black comes off everything, even after a relatively short op. I have a piece which got scrapped anyway because I didn't realign the flip properly, but each side done using the same tool in the same collet in the same nut and the difference in surface finish between the two sides is incredible. The difference being when I first inserted the tool for the first side I forgot to clean everything up first. I will dig it out the scrap box tomorrow and upload a pic as it's a great example.

Here's two pics from different angles. Again this was the same tool in the same collet in the same nut running the same g-code file. Only difference being on the top half (first op) I forgot to clean everything when changing the tool. For the lower half I took the tool out and cleaned everything up.

Quite a difference!!

Attachment 23075Attachment 23074

Thanks for all the info.
I have been using the tool bit to touch off for a while and get okay results. Was hoping the probe would be better and faster.

I have 2 holes in my soft jaws to use as touch off points. I might try and use that method instead of touching off the edges.
The ProbeIt thing is acting up though with the auto probing. Probes something then fucks off somewhere....


Trying to use this bit to make my Fillets. https://www.shop-apt.co.uk/corner-ro...ide-45hrc.html
I am not 100% on the Fusion tool library and can't find examples for this sort of tool.

https://s1.postimg.cc/33kdp5mgcv/Capture.png
NOTE, Diameter is set to 1.3mm and shaft to 8mm. This image is old.

I got it to work though it was either too close to the part on the XY or too high on the Z. Not used it in over 2 months.
Any ideas?



I'v been cleaning mine out too. Not noticed any difference though I have not been looking.
For me it gets clogged up in the collet so when removing the tool I blast it.


[edit]
Think I got it working now. Though speeds and feeds are probably wrong.
Lots of chatter.

So I just used the probe and by hand found the center of one of the button holes in my case.
Was then able to chamfer the edges.
Not bad, not great. Was a hair out on the Y. X was perfect.

I just added 0.025mm to the Y and it is near perfect.
So Zeeflyboy your method works... :p

The real test would be machining around my part top and bottom now with out much, if any step in the surface finish once flipped and had the same operation done.

I guess the best way to do the flip is to leave 0.0something on the bottom of my stock and then flip, then remove that last 0.0something and chamfer...?

Quote:

---

Originally Posted by JOGARA

So I just used the probe and by hand found the center of one of the button holes in my case.
Was then able to chamfer the edges.
Not bad, not great. Was a hair out on the Y. X was perfect.

I just added 0.025mm to the Y and it is near perfect.
So Zeeflyboy your method works... :p

The real test would be machining around my part top and bottom now with out much, if any step in the surface finish once flipped and had the same operation done.

I guess the best way to do the flip is to leave 0.0something on the bottom of my stock and then flip, then remove that last 0.0something and chamfer...?

---

How deep is your case to cut in one pass? I don't think you will ever get this machine to flip a part and cut from both sides without leaving a step, but you should be able to make it small enough to sand and polish out.

Just to give an idea of the machines repeatability I zeroed in on the reamed hole mentioned above, moved my coordinate system over to the vice, milled out a part that was ~1hr machining time, came back to the reamed hole and it was 0.045mm out in Y and 0.02mm out in X.

You should be able to get the results you're after without probing everything. If this is something you're going to be making multiples of it would be well worth your time in making a proper jig.

Quote:

---

Originally Posted by Snapper

How deep is your case to cut in one pass? I don't think you will ever get this machine to flip a part and cut from both sides without leaving a step, but you should be able to make it small enough to sand and polish out.

Just to give an idea of the machines repeatability I zeroed in on the reamed hole mentioned above, moved my coordinate system over to the vice, milled out a part that was ~1hr machining time, came back to the reamed hole and it was 0.045mm out in Y and 0.02mm out in X.

You should be able to get the results you're after without probing everything. If this is something you're going to be making multiples of it would be well worth your time in making a proper jig.

---

I have worked out that I don't need to do the flip on the outside.
I will just use the super glue method to stick my stock onto some sacrificial that I can reuse.
Adds a bit of work removing the glue but it has worked since day 1.

Flipping the part and milling the rest would have meant not spending time on that but it works, don't fix it.


At the moment I can make 2 cases at once. I'd rather not go beyond that as it is more setup and I just need to start making these things now.
Can't spend any more time trying to make it better for batch production...

I have got it to around 3 hours total per pair of cases (not including the rear of the case, though a pair of those are 30 mins.
I can probably get it down 10 mins just with less cautious lead in and lead out distances.
Most of the time is spent with my 6mm roughing bit. That takes out 95% of the material and totals nearly 2 hours of 3.
I have found that I can cut 2mm depth quite well at 75% of the feed it is currently doing (currently 1mm DOC) with my 6mm rougher, so putting adjusting that will result in less time too. Not much but another 10 mins off.

In total I a have 100 of 2 different case designs to make. At this rate I can make around 6 every day.
But for vast majority of that time I will be working on other things (tumblring, PCBs, Anodising, Finishing etc) while keeping an ear on it so it is not that bad.

Just looked back through the thread for pics. I have a suggestion.

First, it looks like your buying custom cut plates? If so, order them cut to size, they always come cut slightly oversize, so rather than milling all that away from the edges, you would just be trimming a mm or so off each side saving you in both material costs and machining time.

Second, you could make a fixture plate for accurate location after flipping. Carry on machining out the guts inside on your vice, in the pic below the three holes circled you could drill out .1mm undersize, hand ream them to size, then use dowel pins in these holes to locate into the fixture plate. These dowels will also pretty much hold the part in X and Y, with a bolt through one of the big square holes and a large washer just to keep everything dead still. Then you can profile round the edge and chamfer or radius your top edges. When it comes to do the square hole which you have a bolt through, just have a pause in your toolpath and move the bolt over to a different hole. This would then also give you the ability to pull a case off and put a new one on without having to rezero, you could also run a toolpath on all your cases in a row, saving you the need to keep changing tools. If you have more than a couple of these cases to make, it would be well worth the price of a 10mm slab of ali and the hour or so it takes to draw up, machine and fix in place. And also far preferable to dealing with super glue.

(Ok it won't let me upload a pic for some reason, but there's only three holes I can see so you should get the idea)

So I finally got that grounding issue message. Guessing I just ground the spindle with the box of the controller?

Pretty much. I just ran an earth cable from a bolt at the back of the frame to the box and earthed everything at that point. It was sticking a CY cable on the spindle that solved my problems.

Looks like it fixed that issue. Odd how all of a sudden that came on.

In other news, Y keeps getting off by a few 0.1s of mm.
X has been fine. This was after 4 hours of roughing out.
Can see on the walls of these two cases that one is thicker than the other.

https://s1.postimg.cc/59idb6qtcv/IM..._190434827.jpg

So after yesterday's work I think I worked out how I am ending up with this problem.

Pressing the STOP button on the remote results in whatever axis is moving to end up being 0.01-0.2mm off where it thinks it is.


Using the pause button is not having the same result from the looks of it.


What I need is for it to not go all the way back home after each OP because that is also resulting in it being out by a few 0.01s over time...

[edit] Will just edit out "G28 Y0 X0"...

So I am having much better luck today.

The probe is 0.1-0.2mm out on both X and Y but I think I am starting to see a pattern so should be able to just offset it next round.
Did end up with 0.2mm out on the Y with these cases but they are not being sold.

https://s1.postimg.cc/2atq3uqmen/IM..._153244374.jpg


I keep getting this bump on the Y face. It is only a hair deep but you can visually see it and feel it.
It is where the operation starts and ends so I am guessing it is something to do with that, not having enough overlap to smooth it out if the bit is coming off the part too quickly?

https://s1.postimg.cc/74ikzza8wv/IM...449825_HDR.jpg
https://s1.postimg.cc/2w3dq5i2of/IM..._163624223.jpg




My soft jaws work really well for holding the cases. Though these were milled back in the day and are not level any more. Probably because I removed them and put them back.
Don't think my vice is all that accurate as well, it not being a proper machinist vice does not help.
I wanted to get one but even on eBay they were £500 for the width I need.
As you can see in the second photo, they result in the chamfer being messed up on one of the edges.

https://s1.postimg.cc/6j8xdog0bz/IM..._153657104.jpg
https://s1.postimg.cc/1igum48qdr/IM...556072_HDR.jpg



Was able to do a nice chamfer on the button and other front face holes for electronic components.

https://s1.postimg.cc/6xfd4joycf/IM...737606_HDR.jpg


Oh and instead of milling out 2-3mm of my mounting holes which I then had to go drill deeper anyway.
Used the chamfer bit to spot the holes so I can just do them on the drill press.
I was already doing them anyway as my 1mm endmill is only 5mm long and I need a few more mm depth.
Other holes like the big one in the middle needed to go all the way down which I can't do with a 3mm endmill that is 5mm long. Do have the 15mm long one that would work but rather just drill it with a 4.5mm that use machine time and an expensive bit...
Obviously the chamfer bit is not made for this, will be swapping it out for a spot drill bit once it arrives.
I have looked at drilling with the mill. I tried it but got horrid results. Though it was probably down to bad setup. Not sure if this machine is really capable of drilling though. Thoughts? https://www.shop-apt.co.uk/carbide-d...d-series-.html
https://s1.postimg.cc/6j8xdog0bz/IM..._153657104.jpg






[edit] Just taken out the parts from the vibratory tumbler and they are looking great.
Really love that thing. They go in for 4 hours and come out great.
So smooth even with some sharp edges. Shame it is such a pain to clean out, not done it yet but that drain port I need to fix...

Nice you're getting there now. For that bump on the Y that's your lead in for your contour, change it so that it sweeps into the cut instead of just moving directly into position.

It can drill fine anywhere up to 8mm I find. 6mm and below it goes through like butter nice and quiet and makes nice long stringy chips. If it's a size you use often it's worth getting carbide drills as you can spin them faster, get them under a bit of torque and also don't need to spot drill first with them either so it saves a bit of time.

Quote:

---

Originally Posted by Snapper

Nice you're getting there now. For that bump on the Y that's your lead in for your contour, change it so that it sweeps into the cut instead of just moving directly into position.

It can drill fine anywhere up to 8mm I find. 6mm and below it goes through like butter nice and quiet and makes nice long stringy chips. If it's a size you use often it's worth getting carbide drills as you can spin them faster, get them under a bit of torque and also don't need to spot drill first with them either so it saves a bit of time.

---

Well I have 1.2mm, 2.5mm, 3mm and 4.5mm holes.
Would it be able to do 1.2mm at something like 5-6mm depth?

Any info on this you know of? Bit scared about Z movement still.

The smallest I have used in ali is 3mm, which was fine. You can drill as long as your flutes are, peck cycle is easy to set up for deeper holes (linking tab on the drilling op in fusion) I generally do to 2/2.5x diameter then use a peck cycle.

I'm not sure what you mean about Z movement. But for as small as 1.2mm I would think a properly trammed spindle would be pretty essential. I can't see why it wouldn't do 1.2mm to 6mm depth, in fact I think the spindle would quite like it as a drill that small will be able to spin pretty fast and won't generate much force. For so many different sizes though you have to weigh up time saved having the machine do it vs time swapping collets and touching off tools. As you said you're making 100 odd, I would be tempted to make a jig with the machine to put the parts on and just drill all the holes with a cordless.

I'll stick with the drill press then.
Wonder if these carbide bits will be better than my hss that I am currently using.
Sometimes the 1.2mm breaks so over 400 holes I am going to go through a few.

That or I do do it in the machine and use my soft jaws.
Might test repeatability tomorrow.

I wouldn't use carbide bits on a drill press, particularly not that small. Your chuck likely has a fair bit of runout and carbide will snap in it like a digestive biscuit.

Quote:

---

Originally Posted by Snapper

I wouldn't use carbide bits on a drill press, particularly not that small. Your chuck likely has a fair bit of runout and carbide will snap in it like a digestive biscuit.

---

Good point.


Not having much luck today.
1 HSS and 1 Carbide down so far and I have only been in the shop for a couple hours -_-

Gives me an excuse to buy some more bits.
Grabbed a 1.2mm for my M1.6 tapped holes (probably swap for 0.3mm as M1.6 holes are meant to be tapped at 1.25mm not 1.2mm).
Also got a 2.5mm for my M3 tapped holes and a spot drill.

Not sure what is going on here.

I have not used the machine in a few days, like 5-7 days.
When I go to home all the axis the Z does not stop when it hits the end stop.

Forgot how I fixed it last time it did this about 1.5 weeks ago.



Also, sometimes when I set my part offsets and then tell it to go to the part's zero, the Z will go about 5-10mm below the set Z. I then tell it to go to zero again and it lifts Z to the correct height.

[edit]
Why is it also normally open? Would have thought NC would be safer?

[edit2]
Gone into diagnostics and all but the Z axis limit switches are working.
The switch its self is working so guessing cable problem.

[edit]
Yea it is cable..

I have the same thing with the go to zero command, always goes to Z-5, I just don't use it and use g0 x0 y0 if I ever need to go there for any reason. Keep meaning to look in to it but always forget.

Having some trouble with Fusion and I have no idea what is going wrong.

For some reason my heights are all over the place and is taking away too much stock on the Z.

Here is part of my case, in RED is what it is meant to be, and in BLUE is what I am getting (using my cheap caliper but it is pretty close to accurate).

https://preview.ibb.co/hORGdG/Capture.png

I am using 3D adaptive clearing for the inside of the case, I set the bottom of the operation on the face of my part at the bottom. This is 2.5mm above the bottom of the stock (I have just switched to +2.5mm bottom stock instead of face selection). I then have another 3D adaptive to clear out the holes at the bottom of the case (I do this because I leave stock and then clean it up using a 3mm carbide).

https://preview.ibb.co/im9mdG/Capture1.png
https://preview.ibb.co/fYeV5w/Capture3.png

Both operations are the same, just different heights and stock to leave.
https://image.ibb.co/nHqysb/Capture4.png
(All my heights are .0mm or .5mm I don't have any heights that are .1mm other than telling it to go 0.2mm lower than the stock bottom for clearance reasons later in the setup)

Any ideas?

There are so many things that could be causing this.

Are all those top surfaces cut by the same tool in the same set up? I can't see how you're cutting 1.7mm too deep from the side wall to the pocket surface, but then the pocket surface is only 1mm deeper than it should be compared to the bottom surface so I think this is a set up error. If you're sure you're setting your Z height accurately, its probably an error in the heights or stock to leave.

Quote:

---

Originally Posted by Snapper

There are so many things that could be causing this.

Are all those top surfaces cut by the same tool in the same set up? I can't see how you're cutting 1.7mm too deep from the side wall to the pocket surface, but then the pocket surface is only 1mm deeper than it should be compared to the bottom surface so I think this is a set up error. If you're sure you're setting your Z height accurately, its probably an error in the heights or stock to leave.

---

There is no stock to leave. Z height is all the same for all the operations.
I am using the 6mm roughing bit for most of the milling on this part. It does all the surfaces too.

I just ran the operation again but specificity all the heights manually from stock bottom and now it is just 0.3mm out.

The towers are all the correct height which is okay. But the bottom being so far down means my PCBs don't sit and the part that sits in the curved section is not being clamped down, it is just lose as there is 0.6mm too much Z.

This is definitely something in my Fusion operation.


I do have the minimum Z DOC at 0.5, so why it is cutting down at something not divisible to that, idk..

Is your Z axis calibrated correctly, and not gaining/loosing steps?
I'd double check the calibration, then mark the z-shaft, create a program that runs the Z up/down a hundred or so times, and check it's returning to the same mark.

If that reveals nothing, try modelling and machining a simple stepped block, to see if it's a fusion or machine problem.
While machining pay attention to where the mark on the shaft is at a known position, then return to that position at the end to see if anything has moved.

Quote:

---

Originally Posted by m_c

Is your Z axis calibrated correctly, and not gaining/loosing steps?
I'd double check the calibration, then mark the z-shaft, create a program that runs the Z up/down a hundred or so times, and check it's returning to the same mark.

If that reveals nothing, try modelling and machining a simple stepped block, to see if it's a fusion or machine problem.
While machining pay attention to where the mark on the shaft is at a known position, then return to that position at the end to see if anything has moved.

---

This has only been a problem with the last 2 setups I have ran.
All the ones before executed as expected.

If you have your heights set up accurately, where do you have your part located in the actual set up? Fusion automatically sets the part in the centre of the stock and you have to change it manually. If correct...

How are you setting your Z height? If using the Z setter I tested that quite a bit one day and got errors anywhere up to 0.3mm even using a slowed down double probing routine, its just not consistent for some reason, or at least mine isn't anyway. I don't use it anymore and touch off with a feeler gauge which takes a little longer but is far more accurate and repeatable.

Also the original hollow panel OMIO bed is a block of turd to put it lightly, putting a sheet of A4 paper on it will probably cause it to deflect. Getting smooth top surfaces and accurate heights is nigh on impossible, so expect to see a bit of error. I got a big slab of aluminium tooling plate to replace it and the improvement is massive. The last part I made was meant to be 12.55mm high and came out at 12.54mm with both surfaces flat to within 0.00mm and smooth to the touch. An impossible task on the original bed, its an addition worth its weight in gold imo, well worth looking in to.

Quote:

---

Originally Posted by JOGARA

This has only been a problem with the last 2 setups I have ran.
All the ones before executed as expected.

---

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