CamBam
News:
 
*
Welcome, Guest. Please login or register.
Did you miss your activation email?
May 22, 2019, 13:37:37 pm


Login with username, password and session length


Pages: 1 ... 5 6 [7]
  Print  
Author Topic: Automatic tool changer for the lathe  (Read 20128 times)
dave benson
CNC Jedi
*****
Offline Offline

Posts: 1087


View Profile
« Reply #90 on: November 24, 2018, 23:18:53 pm »

Another small update

In the picture, is a small test piece that was done with fusion 360, previously I've been using the wizards in Mach3, which on the whole have been good to work with and for more complex tasks.
I've been using Ezilathe and importing the .dxf from CB and producing a file.
In this file I've selected CSS (constant surface speed) and tried to get most of the operations done with the Gcode

I made a mistake with the OD by selecting too small a cut for the finishing pass, the original depth of cut for the roughing pass produced a far better finish.

The ID boring went well and the sizing for the bushing was good.
The job was mainly to get fusion to produce Gcode that worked with the turrets.

What I found was with (using the wizards and Ezilathe) I needed a G53 in the Tool Change Macro.
But with fusion this wasn't necessary and I had to remove the G28's But all in all it wasn't too bad.

It’s funny you know, I've got six tools now to choose from, but more would be better, so in the next few weeks I think I'll make a Gang tooling post  to hold a centre drill and some smaller sized drills up to 6 or 8 mm, as the aim of the game is to get the lathe to do as much as possible of the work.

Dave


* Inner bore at CSS from fusion.png (145.73 KB, 388x218 - viewed 60 times.)
Logged
dave benson
CNC Jedi
*****
Offline Offline

Posts: 1087


View Profile
« Reply #91 on: January 03, 2019, 21:42:33 pm »

Another small update.
Santa delivered a Bandsaw for Xmas (I love Santa) They are sold here as a Saber bandsaw (someone forgot to take out a few references to Grizzly in the manual though Grin)
Mechanical Hacksaw cut time 17 mimutes for a piece off 130mmx12 mm thick  Bandsaw ---> 7 and a half minutes.

I've ran this particular Turret for 3 or four weeks now, and am on the whole pretty happy.

I did part off a few Indexer Bases (I've had mixed results with the Tool in the tool post) and the job cut like butter.

I had some feedback stating  that it would be nice to (when setting the tool height after a crash) not to have to
release the indexer manually through the interface as this step could be forgotten and while leads to no damage
could (has) lead to the indexer moving as the overload bolt is secured and then must be reset which is a pain in the butt.
My first thought when this was mentioned was well don't forget, but after thinking about this for a few weeks
and watching a video about (Lt Murphy) from  Murphy's law  fame. he was a real guy and I discovered that even
Wikipedia had the commonly stated version of this law but this is not quite right. sensor plugs on a manned rocket sled should be polarised

Anyhow I decided to eliminate the step of manualy releasing the indexer, and so redesigned the Indexer completley and have a test turret where you don't have to do anything just set the centre height and tighten the bolt.

It is a Twin Pawl mechanism with automatic wear compensation and should not have to be adjusted for the life of the turret.
I had origionaly wanted to do this, but could not figure out how to do it. This time it was easier as I had spent
a lot of time on the turrets and watched thousands of tool changes.
Dave


* Turret Dec 30 2018.png (2113 KB, 800x1422 - viewed 63 times.)

* New Band Saw.png (1106.22 KB, 563x1000 - viewed 90 times.)

* Turret Twin Pawls.png (1993.62 KB, 800x1422 - viewed 69 times.)
Logged
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3568


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #92 on: January 20, 2019, 17:48:55 pm »

Some nice work Dave.  I say Kudos to finally getting a horizontal bandsaw.  I remember when I got my first one.  A little 4x6 Harbor Freight unit with just gravity feed and a spring to relieve over pressure.  Its another machine that can work FOR you while you do something else.  I have since picked up a 7 x 10 with pneumatic feed control, but I still have my 4x6 attached to the end of a roller table.  When I made my very first bandsaw cuts I was ecstatic. 

That sneak up to dimension on the finish pass has bitten many a lathe operator.  With my limited knowledge base I have found (manual turning) that I get the best results by varying depth of cut and feed rate until I find the right one, but before I get to dimension.  When I get a good finish I mic, take another identical cut and mic again.  This tells me to finish to the dimension oversize that allows me to take the right final pass for a good dimension and finish quality. I don't have enough experience that I would have enough confidence to go straight to CNC with a turned part.  I think if t was a massed produced part I'd either CNC a couple prototypes and then go back my CODE to make adjustments before starting the production run, or I would make one or two pieces manually and take notes to use when I coded the part for the production run.  

Again, very nice Dave.  
« Last Edit: January 20, 2019, 17:52:03 pm by Bob La Londe » Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
dave benson
CNC Jedi
*****
Offline Offline

Posts: 1087


View Profile
« Reply #93 on: January 21, 2019, 06:50:23 am »

Thanks Bob

Yeah, getting the Band-Saw has made life much easier, the machine is built with much better quality standards than the Lathe
I bought perhaps 10-15 years ago. I really (to and fro'ed ) over getting this one, or a bit bigger one (like David's), and finally decided
on this one because, I wanted to do vertical cuts as well as horizontal.
 
This has helped on some parts (cutting vertically that is), where I've more or less cut the part out, close to the final dimensions on the Band Saw
and cut at full depth using the shrinking toolpaths strategy with a fixture. 

I've no complaints it works well and is quiet and fast.

As to the Lathe making good parts, I start off by taking a test cut and measuring with the Mic and checking that with the DRo's.
Indicate X and Z in. as I'm mostly using Carbide tooling, I've found that there is a minimum depth of cut for these, so what I do is
arrange the cut order so that on the final cut, I've got enough meat to cut and get a good finish.

In Fusion you can also specify the number of spring cuts, which varies with the stock Dia and the amount of stickout from the chuck
or whether the work is supported or not. This is mostly knowledge gained from trial and error.

In general I try to get "C's and 6's" from the cut and this pretty easy to get, because I set the feedrate and
then adjust the RPM's to suit. Then use these values in Fusion as a guide and sometimes adjust these slightly
at the Lathe.
I've been experimenting with CSS constant surface speed lately, and will be incorporating this into my code from now on.
I've found it an order of magnitude easier to hit tolerances with the lathe compared to the Mill.

Bob, once you have CNC'd the lathe, you won't look back, for me what makes using the lathe so enjoyable is that it's very repeatable
so that you can set up a file say for a 12 mm thread from 16 mm stock for 15 mm length in 1018 sticking out perhaps 25 mm from the chuck.
I made a file for this and other thread sizes with the Mach3 wizards with a spring pass, so now I put the work in the chuck and touch off
make sure the turret is turned on (3 tool changes) press the button and walk away and do something else and when the machine stops
go and get the parted off stud.

I do this on a regular basis for different stud sizes and it just works. the biggest thing is to not get stringy chips
if you can get your chips, if not "C's" and "6's" at least a manageable size then you can leave the machine to make the part and do something else.

What I do for ID boring for a bearing is use the carbide boring bar to rough (biggest cuts I feel comfortable with)
to almost size and then use the Hss boring bar, and sneak up on the size often at this stage I let the material cool back down
to ambient temp before measuring and taking the final cut.

I've received the ER11a collet chuck and when I get time, I'll make a gang tooling post. well put it the ToDo list anyway.

Dave
Logged
dave benson
CNC Jedi
*****
Offline Offline

Posts: 1087


View Profile
« Reply #94 on: January 21, 2019, 06:53:53 am »

What's happened Lately with the twin pawl setup, I have mechanism going now, although it's been a tale of frustration and woe really.
What I discovered while assembling and testing was that the two pawls were not identical close but no cigar as when they were put
back to back and indicated concentric, some of the pawl teeth did measure up (I discovered this as the secondary pawl is operated by a cam)
of 1.5 mm throw and it's angular position when the pawl is locked up,is a good indication of how accurate the machining was at each tooth of the pawl.
When I did the Z Axis upgrade, I also checked the Y axis as this one showed up as the culprit when I did the drilling and machining tests a while ago, and replaced the motor couplers with solid ones.
 
I didn't know what to do for a while as I've checked the Y Axis many times and it always seemed ok, then I hit on an Idea and placed the Z Axis resting on a bit of wood on the machine vice and stalled the motor out, and saw that I had at the top of the Z Axis column 0.07 mm movement in the Y direction.
 
because this was late at night I found a bit of heavy wall 2 inch tube about 3\4's as high as the column and made a temporary brace, I was now down to 0.03 movement.
 
The next day I made a brace out of some 130 mm x 12 mm 1 m flat bar, and then made a new pair of ratchet wheels, and while not still not perfect
are within, (I'm guessing) perhaps 10 degrees  on the adjustment cam which (because of it's small throw tends to amplify the error so it's easy to see).
The allowable limit for the mechanism to work is at around 80 degrees + or - 5 degrees so that it can't be back driven.

I also had to heavily modify the Gcode by putting the machining tabs in strategic places where they were easy to cleanup but provided enough support for the following mops.

And in the first profile mop using an extra bit of cutwidth to help clear the chips as well as a second finish mop at full depth (tangent leadin)
and then using the collision detector to clean up the root of the teeth  with a 3 mm end mill (3 mops per tooth each with different Roughing clearance ) to sneak up on the size and not overload the endmill.
I then did some hand optimisations to stop unnecessary moves to the clearance plane.

Two thing's I noticed while doing this file were:

I had a lot of copy and pasted mops where I wanted to change only one or two of the values, and this took quite a lot of time.
I'll look into this when I have time.

When Coping a profile mop (6mm EndMill that had Machining Tabs) and then changing the diameter of the endmill and regenerating the code for a 3 mm endmill
the size of the machining tab changed (got smaller) and as this mop ran directly after the previous one (with a wider machining tab) it would have most likely broken the cutter.  So something to look out for and adjust when necessary.


Dave
Logged
dave benson
CNC Jedi
*****
Offline Offline

Posts: 1087


View Profile
« Reply #95 on: March 18, 2019, 03:43:28 am »

Another small update.

Well after doing all that work on the machine, I set out and made some more secondary ratchets, two at first and measured them.
They were both identical two each other, but unfortunately were still 0.07 mm out in the Y Axis, which gave me the irritations no end as I thought I had fixed the problem.
I then removed the table, stripped the whole thing down removing the ball screw and the Ball-screw bracket that attached it to the table and finally found the problem.

The Ball screw bracket is attached to the table with a tapered spigot (with an M8 bolt), I'd checked this many times as its  easy to do and it was always tight.
It turned out that the spigot (cast iron) had a hairline crack about half way up, which meant that when I checked it, it was tight but the bottom half of the spigot, which was still attached by the bolt threads and captured in the tapered hole could move a small amount.

If I hadn’t taken the table completely apart I don't think I would have found it.
Anyway I re-did the Secondary Ratchets and they work well now on the workbench test turret.

I did some more work on the Auto tool identification, and it turns out to be relatively straight forward accurate and repeatable.
I have begun to look at the Auto tool touch off feature and as usual (The Devil is in the detail) as two cameras would be required both running without IR filters.

The last item on the list is compensation for tool wear, and also for setting a new tools offset in the tool table automatically.
This looked like a mission impossible for a home gamer, until I saw a guy on  you-tube hack a older type laser diode and use it for Interferometry.

Part way through the video I realised that I could apply this technique to this problem, And I'm sure that you could have heard my jaw drop half a block away.
After looking at the rest of his videos as far as I'm concerned this guy is in the Genius category.

Dave


* Cracked table Spigot.PNG (118.81 KB, 675x581 - viewed 26 times.)

* Correct Tool Identification.PNG (419.21 KB, 609x329 - viewed 41 times.)
Logged
EddyCurrent
CNC Jedi
*****
Offline Offline

Posts: 3924



View Profile
« Reply #96 on: March 18, 2019, 10:32:45 am »

Dave,

Maybe the tools could be barcoded ?
Logged

Made in England
dave benson
CNC Jedi
*****
Offline Offline

Posts: 1087


View Profile
« Reply #97 on: March 18, 2019, 12:38:41 pm »

Hi Eddy
I'm sorry, I didn't make myself clearer, it's sort of buried in too long a of a post.

The blue square in the picture indicates a positive match between the image stored in the plugins
tools dir and a tool that would be in the turret tool slot.

This particular method is called feature mapping and  uses a technique called 'Speeded Up Robust Features'  SURF for short.
The really good thing about this approach is it is scale and angle invariant meaning that the tool can be found even if the
camera is of at an angle from the turret or is up close or far away.

This part of the turret software works accurately and repeat ability, and has not failed once to identify a tool.

There are other approaches to identifying objects for instance Colour and Shape and Outline, Bar codes QR codes ect, but I found these methods to be less than optimal and as this process is critical to the to the turrets performance it has to 'Just Work'.

One fly in the ointment was that some of the surf routines are patented, so it took  a very long time to find an open source alternative that was bullet proof.

When you first install the turret, you teach it what each tool looks like by selecting each tool that telling the turret to take a picture of the tool and entering the tool description (the same as the description in the tool table in mach3)  and then every new tool from then on.

For example as  Mach3 is running a Gcode program, it may call for tool  number one  (in my case this is a Right Hand Turning insert tool) and after the turret has changed the tool it will check that you have indeed a Right Hand Turning tool in that particular tool slot, and if the tool turns out to be a Boring Bar or something else then the turret will
cycle through the other tools looking for a Right Hand Turning Tool  (you may have just placed it in another tool slot) and if it finds the tool it will use it.
Else it will stop the lathe and flag an error and wait for you to put the correct tool in the tool magazine.

This is the stage I'm up to now and am very happy with it, the next stage is to do Automatic Touch Off which is quite a big deal (difficult to do)  along with tool wear measurements using interferometry.

The only other thing I would like to look at is temperature compensation , for example if I have to whittle down a lot of material in preparation for something critical like a bearing fit then I have to leave the job until it cools back down to ambient temp before measuring it again to get the correct size.

There is a Kickstarter project where they have a camera that can take a Fleur lens (and is not that expensive) with which I could take an  accurate temp of the workpeice.

 Dave
Logged
dave benson
CNC Jedi
*****
Offline Offline

Posts: 1087


View Profile
« Reply #98 on: March 26, 2019, 12:52:22 pm »

Another small update.

I've been doing some more testing of the vision capabilities of the software, and in the pic below
ran a test with a cheap $8  webcam hand holding it above the test turret inside, and it seems pretty
 able to detect the tools even though my hands were a bit shaky and the image is a little out of focus
because of this and at 70 to 80 deg to the origional picture orientation.

I'm now in the middle of making a rack to run along the lathe for the camera to sit on, and have ordered a
middle of the road camera from Microsoft.

I've also purchased a new lathe chuck, a 160 mm four Jaw Independent, as the one that came with the lathe
is terrible, just have to make a Backplate to suit the spindle 39x4mm thread.

I've also looked into the measuring tool wear thing, and there are quite a few issues to overcome some electrical
(High gain Opamps and filtering)  and although I plan to be measuring an order or magnitude less (maybe two) then Ben over at the Applied Science Website.

And some mechanical details as well. I sorta guess that I've have trouble keeping the vibration at bay while staging the sensor. Anyway I've ordered some Sony laser diodes (the one's Ben  is using and pointed to ) are getting long in the tooth.

There were still some at Jamco and Amazon and one box of one hundred on Ebay, but I've managed to find these
which are a bit more plentiful and cheap.

Dave


* finding out the limits of tool detection.PNG (564.81 KB, 813x306 - viewed 31 times.)

* new 160 mm 4 jaw independent chuck.png (838.91 KB, 640x480 - viewed 21 times.)

* new turret camera.jpg (2.21 KB, 140x140 - viewed 163 times.)

* sony sld3232vf laser diode with pin diode for feed back.jpg (2.24 KB, 140x140 - viewed 161 times.)
Logged
dave benson
CNC Jedi
*****
Offline Offline

Posts: 1087


View Profile
« Reply #99 on: March 30, 2019, 08:26:03 am »

Another small update.

The camera turned up a couple of day's ago, and on the whole am pretty pleased with it.
It did take some time to set it up correctly for this task, and I've done many tests with different
settings for resolution frame rates,auto-focus ect, It was a lot of fun chasing the optimum settings
down, but to keep the thread short won't go into the detail's.

I've made a new tabpage where you can set up and test the camera at the lathe for different lighting,
and camera positions.
You can elect to use the computer vision or not.
If you do, then you must teach the turret what each tool looks like using the capture tool button
and save it to the turret tool dir.
At the moment if the turret finds the tool slot empty or another tool in place of the required one
then it will stop and wait to operator input, but I will code for it to either look for the tool in another slot and if
it finds the tool then adjust the tool alias table and continue on with the job .

I'm going to put the coding aside for the moment as I've bought some HRS 200x200x16 mm plate and a
piece of 1040 75 dia x 100 long round bar to make the backing plate for the 4 jaw chuck.
and plan to make a boss and press it into the plate and machine it, and then drill the mounting holes
on the mill.

Dave


* tool teaching.PNG (247.95 KB, 424x634 - viewed 32 times.)

* Tool ID Success.PNG (103.66 KB, 433x697 - viewed 29 times.)
« Last Edit: March 30, 2019, 08:32:00 am by dave benson » Logged
dave benson
CNC Jedi
*****
Offline Offline

Posts: 1087


View Profile
« Reply #100 on: April 19, 2019, 11:15:08 am »

Another small update.
I used the twin pawl setup now for a couple of weeks, and it has performed well, as it locks the turret plattern rigidly.

I did have to ditch the solenoid activation as this new mechanism  requires more force to operate.

I tried very hard to keep using the solenoid activation method, as I was trying to make the turret as a whole
simple and robust, and if anything did go wrong it would be cheap to fix with easily available parts.

However the solenoid would have required a torque multiplier (like the capstan in the original indexer)
adding to the mechanisms complexity,cost and extra failure points.

So I Servo'd the secondary pawl, which added to the cost (10 times the solenoid cost) it proved to be a great boon though
as the energy budget required dropped significantly.

The Idle current has gone from 286 ma to 113 ma giving about 55 hrs. to remember that you left it on.
This had nothing to do with the servo but rather turning off all the peripheral clocks not needed and a few other power saving tweaks.

The number of tool changes has increased from 720 @ 18c to 1600 @18c using the same test procedure.

This was mainly brought about by not wasting power to energise the solenoid during the whole of the tool change
as the servo is used only open and close the latch. I also was able to add another 18650 cell to the battery pack
as the original indexer was in a different position preventing me from doing so.

I can't test much at the moment on the lathe as I've started to install a ball-screw like Steve has done with his build
and have machined the saddle and made some brackets, just waiting for a bearing block for the front support.

The laser diodes have not turned up yet, and I may have made a mistake as I ordered 405 nm ones rather than the 625 nm ones Ben used and on the weekend will talk to friend who ran his own a laser company for many years to see what his opinion on the viability of this Idea is.

Dave


* 1600 Tool Changes.PNG (91.48 KB, 413x690 - viewed 19 times.)
Logged
dave benson
CNC Jedi
*****
Offline Offline

Posts: 1087


View Profile
« Reply #101 on: May 11, 2019, 02:51:24 am »

Another small update.

I had a long talk with my Laser friend and, at the start of the conversation we discussed the challenges of the project.
Noise in the system both mechanical and electrical and these will be challenging.

We reviewed the video Ben did again, and downloaded the white papers, where about half way through the paper there was
an example showing a milling machine where they were applying one of the three possible techniques that can be used
with the essentially the same hardware.

Mr friend Ray pointed me to a supplier he has used in the past and found to be reputable, then we looked at quite a few data sheets
for a suitable laser diode this one -->  Opnext HL6358MG A red laser Diode at 635 nm with the appropriate output.
I ordered two and they came quickly (arrived last week) and were very well packaged.
I also ordered a variable current and voltage power supply module (still not here).
I then whipped up a signal generator for a spare Due I had lying about.

While functional, I don't think it will 'cut it ' for this purpose, so I will order a signal generator chip (MD_AD9833) that I can send signals to via the uart and it will generate the sine wave, leaving the Due to just count pulses.

The big issue as I see it will be mechanical noise from the environment.
I discovered the magnitude of this problem fitting the camera for Auto Tool recognition.
I had placed a ip67 outdoor flood light which I had gutted to fit the camera on a stalk (400mm long) to oversee the tool changes.
the Damn thing when hit with a blow would ring like a bell, so I'm going to have to attach a stabilising strut back to the wall.

Realistically measuring tool wear is a non starter,but measuring tool length and updating the tool table offsets will be do-able.

Cutting the boss with a M39 x 4 mm thread was a complete balls-up as I used a AG60 insert thinking it would be OK, what I got was a fantastic looking thread that would spin on only 3 turns and then lock up, on investigation the insert was only good for up to 3.175 mm pitch threads, so I'm going to have to find another threading  insert that's good for 4 mm pitch threads and have another go at it.

The only good that came of the exercise is now I can pick up a thread with the lathe after removing and inserting the work piece and have learnt about G32 threading.
edit : I also got the Idle current down too 39 ma and could go more but will have to do more fiddling about.
Dave
« Last Edit: May 11, 2019, 02:54:57 am by dave benson » Logged
Pages: 1 ... 5 6 [7]
  Print  
 
Jump to:  

Powered by MySQL Powered by PHP Powered by SMF 1.1.21 | SMF © 2015, Simple Machines

Valid XHTML 1.0! Valid CSS! Dilber MC Theme by HarzeM
Page created in 0.15 seconds with 18 queries.

Copyright © 2018 HexRay Ltd. | Sitemap