Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: andy_con on October 24, 2012, 05:33:53 PM
-
hi all,
ive got a denford traic vmc milling machine which runs on mach3.
ive just received this bad boy -
http://www.ebay.co.uk/itm/230832885828?ssPageName=STRK:MEWAX:IT&_trksid=p3984.m1423.l2649
(http://i187.photobucket.com/albums/x202/magicmushrooms1/12100099.jpg)
can anyone give me any info on how to set it up in mach3?
im assuming i need some fancy code to tell the machine when to pull up etc?
-
Looks like a reversing holder so easiest way (if you have spindle speed feedback) is to use G95 and feed at the required rate for the pitch then reverse the Z at the desired depth.
Hood
-
ok thanks, to be a pain could you explain a bit further?
ive only owned my mill with mach3 for two months so im very very new to all this
i want to tap m2, m3 and m9 holes
-
Ok first thing is do you have spindle speed feedback to Mach? In other words does the RPM of the spindle display correctly in Mach?
If it does then what you would do is change to G95 just before you wanted to start the Z moving down.G95 is feed per rev so you would then command the Z to feed to the depth you want at the feed suitable for the tap.
Example, you would position the tap above the hole then your code would be something like this if the depth you wanted to tap was 10mm and you were using a M3 tap (M3 tap is 0.5mm pitch)
Position above the hole with the code (say 5mm above) then the code for the actual tapping would be
G95
G1Z-10F0.5
G1Z5
G94
Obviously your spindle would have to be running etc but that should be happening with your prior code.
Test cutting air for a while until you are sure it looks fine then test in some soft material. Once you have done it once or twice you wont have to worry :)
Hood
-
many thanks for the detailed information.
not sure on the rpm thing, how would i find this out?
i have to set to spindle speed before i can do anything so command s3000, does that mean anything?
-
If using the standard Mach3 mill screen you will have a DRO that is called RPM, if that you command a spindle speed and switch the spindle on with a M3 or using the screen button then the DRO should start reading the true spindle speed. If it is at zero when the spindle is running then you dont.
Hood
-
ok ive just been told no spindle feedback, is this going to cause issues with using the tapping head?
-
It makes it a bit more hit or miss. You should still be able to use G95 to make the feed calculation easier but Mach would just assume that the spindle is revolving at the commanded speed, if its not then the feed would be wrong.
You could also use G94 (feed per minute) but that means the feed has to be calculated with respect to your RPM and then, as before, it would all hinge on how accurate your spindle speed is in relation to the commanded (or calculated) speed.
With a reversing tapper it should be ok as long as you are close or if anything slightly under feeding the Z as the tapper should free wheel if its going down too slow for the spindle speed. Go way to slow and it will reverse as you are going down which you dont want.
Hood
-
IF you log onto the tapmatic website you will find code examples for their tapping heads (;-) it is a bit different than you think.
Just a thought, (;-) TP
-
Try here for the CNC Gcode example. I have one of those bad boys sitting in the tool crib. You MAY want to double check the oil in the oil for signs of Coolant contamination and change it out if needed.
http://tapmatic.com/images/pdf/install_instructions.pdf
Just a thought, (;-) TP
-
Hi, This is the website for the manufacturer, it looks like and auto reverse is part of the internal actions. By the look of the exploded drawing don't attempt to take it apart.
http://www.smiag.ch/ModuleFiles/Werkskataloge/107/PDFFile2/TIC_Katalog06_engl_081206.pdf
Jim
-
Sorry forgot to say page 33 gives example of fanuc programming.
http://www.smiag.ch/ModuleFiles/Werkskataloge/107/PDFFile2/TIC_Katalog06_engl_081206.pdf
Jim
-
thanks for all the info guys, looks pretty complex.
-
Ag yes forgot that you would need to fast retract the first bit of the reversal to engage reverse or you would overfeed. Other than that the important factor is knowing the correct spindle speed rather than just what has been commanded.
.
Hood
-
so is my understanding of how they work wrong?
i thought you fed the tap towards the hole at a slow speed, when the tap reached the hole you fed down a little bit till the tap bit.
with the spindle travelling at a slow speed when the tap bit, it would just tapping to the bottom of the hole when reaching the bottom reverse would engage and the tapping head would retract and come out. then you just need to pull the tap out.
???
-
I have not studied the tapmatic pdf properly but the normal reversing tapping heads I have seen have a cone clutch arrangement in them, when you feed down the cone engages and drives, when you stop feeding the tap is still pulling down due to spindle still rotating and the feed cone will start to disengange. This is where you do your short fast move to take up the slack to quickly engage the reverse cone and the tap rotates the opposite way and you retract at the standard feed.
The feed is based on RPM and Pitch of tap. G95 makes it simple, especially with metric as all you need to do is have your feed at the pitch of the tap being used. If you are using G94 then you will have to calculate what the feed is to be based on the pitch and the RPM the spindle is doing.
As mentioned though you really need to know the true RPM to make it work correctly as without feedback from the spindle you cant be sure the RPM is what has actually been commanded. Two options, use an external tach to see what the actual RPM is or make up a slotted disc with an opto so Mach gets feedback.
Hood
-
ive been told my machine has spindle feedback but its connect to the spindle drive.
so i need to look into this further
-
Do you have any links to info on your machine?
Hood
-
http://www.denfordata.com/pdfs/triac_series_600dpi_hq.pdf
-
Not a huge amount of info in that, well not the type we are looking for. Understandable as its a user manaual I suppose :)
Anyway if you have a look on the spindle drive you may get a clue as there are inputs to it lower left and info screen printed on the pcb. One may say Index?
Hood
-
I always tap in G95 mode. Makes the math easy on the feedrate. Heck take it apart it is NOT that complicated.
-
There's no need to take the tapping head apart to understand how it works. It has clutches in it. As long as the tap is moving down, the tap will keep turning CW. When the tap stops, the tap will be dis-engaged, and, shortly after, the 2x reverse gear will be engaged, backing the tap out.
Regards,
Ray L.
-
Ray what I was referring to is MANY of the older units I see today need to have the Guts cleaned AND the oil changed in the head. They get contamenated with coolant over time. IF left it may corrode the internals THEN you really have a mess.
The way they work is there is a spring loaded neutral positon. When you downfeed and the tap touches the material it pushed the forward clutch into gear. When you stop the downfeed the clutch releases and goes into neutral. As you do a rapid UP feed it engages the reverse clutch and backs the tap out . The unit is a floated head so a little mismatch on feeds is NOT a big deal.
Using the G95 mode without an RPM index will work fine as long as you are close.
Just a thought, (;-) TP
-
lets see what info i get
http://www.denfordata.com/bb/viewtopic.php?f=47&t=3907
-
Tapmatic has a demo video on youtube showing many different size heads in action with the tap size and RPM listed.
http://www.youtube.com/watch?v=ZGMC55t-98E
-
ONe thing you do have to watch for is doing it their way you can TEAR the top thread when the tap gets to the top of the hole AND it is extended too far the spring back can tear the top thread when i t retracts back to center.
(;-) TP
-
ok i have finally received my spiral taps.
so i can now test the tapping head.
let get down to coding, what do i need to use here?
tap is an m3 tap, the hole is a through hole and say 10mm thick work/or 10mm deep hole
-
Are they spiral flute or point? Spiral flute are really meant for blind holes and spiral point are best for through holes.
With spiral point the chips are pushed in front of the tap and out the hole so there is less chance of the chips snagging and causing problems.
Hood
-
they are flutes, cos once sorted i will only be tapping blind holes.
but for testing i did some through holes
-
The code would just be similar to what is in the tapmatixc manual except personally I would use G95.
Did you ever get info on the spindle speed sensor?
Maybe wouldnt be too hard to add a slotted disc and opto if you cant use whats there?
Hood
-
out of 4 taps i have 1 left lol.
m3 tap didnt work to bad, but trying different things i broke two.
m2 tap broke within about a second
was using g95
-
oh and adding spindle feedback is possible but a right pain in the arse
-
Just looked at your denford data question and looks like you could add a disc to the motor shaft. All it would then need is an opto going into your parallel port. Even if the motor is not direct drive that wouldnt matter as you can tell Mach to divide the index signal by whatever the gearing is.
Hood
-
in the long run yes i could, but it would be nice to get the tapping head up and running now.
need to order some more taps.
only got one m2 tap left
-
MAKE sure you are optimum on the hole size for tapping and are using the correct H# for the tap application. SUper tight fit toleranace on threads do not always make the best thread, usually all you get it is broken taps in an expensive part to fix.
(;-) TP
-
im using a 1.6mm hole for an m2 thread and 2.5mm hole for m3 thread
-
this is what someone has recommended
http://www.cncdoctor.co.uk/index-pulse_62.html
-
Yes looks reasonable and I am sure it will work well. I just used an OPB916B opto and a 220 Ohm resistor and it worked great but suppose its not that much cheaper. http://uk.rs-online.com/web/p/photointerrupter/4550896/?searchTerm=opb916b&relevancy-data=636F3D3226696E3D4931384E4B6E6F776E41734D504E266C753D656E266D6D3D6D61746368616C6C7061727469616C26706D3D5E5C772B2426706F3D313326736E3D592673743D4D414E5F504152545F4E554D424552267573743D6F7062393136622677633D424F544826
Heres a link to the way I had it set up on the Bridgeport. http://www.machsupport.com/forum/index.php/topic,17032.0.html
Hood
-
is there no non contact tachometer set up i could use?
a hand held unit is mega cheap
http://www.ebay.co.uk/itm/New-Digital-Laser-Photo-Tachometer-Non-Contact-RPM-Tach-/220972093324?pt=UK_BOI_Electrical_Test_Measurement_Equipment_ET&hash=item3372f68f8c
-
You could use a manual tach but it would mean to be sure you would have to measure each time you were about to tap to make sure the spindle was turning at the speed your code was telling it to. I would say it would be much simpler connecting up a spindle sensor of some sort, that way you would have a constant true speed reading in Mach and G95 moves would be based on that RPM rather than what you have coded.
Hood
-
Andy, if you're worried about identifying the wires in the loom, just run the existing wire from the sensor into the case
-
ill get the sensor kit ordered and see what i can do.
not fully sure how im going to machine up a disk to go round the spindle
-
for a temporary setup you could tie wrap an actuator to the top of the spindle
-
ill just go with the kit from cnc doctor for now see how i get on
-
ok cnc doctor is out of stock
so hood how do i get one of these working with mach3?
http://uk.rs-online.com/web/p/photointerrupter/4550896/?searchTerm=opb916b&relevancy-data=636F3D3226696E3D4931384E4B6E6F776E41734D504E266C753D656E266D6D3D6D61746368616C6C7061727469616C26706D3D5E5C772B2426706F3D313326736E3D592673743D4D414E5F504152545F4E554D424552267573743D6F7062393136622677633D424F544826
-
Have a look here.
http://www.machsupport.com/forum/index.php/topic,21302.msg148503.html#msg148503
Hood
-
shame maplin or rapid doesnt sell these sensors.
ill get one ordered thanks for the info
-
http://www.maplin.co.uk/photo-reflector-sy-cr102-12709
-
ah they call it something different, good old maplins.
im assuming its exactly the same and wired the same? (electronics is not my fing)
**
A slotted disc attached to the spindle, an Optek OPB 916B optical switch and a 220 Ohm resistor are all thats required. Take 5v from the BOB to the white wire on the opto, take the same 5v source to one end of the resistor and connect the other end to the red wire on the opto. Connect the Green and black wires of opto together and connect to 0v (Gnd) terminal on Bob. Take blue wire from opto and put to an input on the BOB. In Ports and Pins, Inputs set p the Index to the port and pin you have it connected to.
BTW Mach has to be licensed for threading just in case you are in demo and wonder why it doesnt work.
**
-
just got two opb916b's today.
but i forgot about the resistor, is the resistor 100% needed?
also what is the BOB?
-
Yes you need the resistor, if you dont then you will blow the LED as it is needed to limit the current to it. You dont have to be exact with that resistor so if you have any close you could use them.
Hood
-
ok found a suitable resistor.
so is it the blue wire that goes to the input on my break out board?
all help welcome
-
http://www.rapidonline.com/Electronic-Components/Transistor-output-optoswitch-29427
http://www.rapidonline.com/Electronic-Components/Transistor-Darlington-photo-interrupter-68054
-
Yes the blue is the input to the BOB (Breakout Board seeing as I forgot to answer your previous question ;D )
Hood
-
excellent thanks.
i got two sensors just incase so fingers crossed
-
sorry what are these? do i need them?
http://www.rapidonline.com/Electronic-Components/Transistor-output-optoswitch-29427
http://www.rapidonline.com/Electronic-Components/Transistor-Darlington-photo-interrupter-68054
-
more sensors, these are from Rapid.
-
oh right but i dont actually need them if i have the other sensors?
i didnt get round to wireing tonight as i made one of these from scratch again -
(http://i187.photobucket.com/albums/x202/magicmushrooms1/cnc/12110007.jpg)
(http://i187.photobucket.com/albums/x202/magicmushrooms1/cnc/12110008.jpg)
could i just confirm before i wire tomorrow
so i apply 5v to white wire of sensor
add resistor then 5v to red wire of sensor
connect green and black wires to 0v or gnd of 5v psu
connect blue wire to input/break out board?
-
Connect one end of resistor and white wire to 5v. Connect Red to other side of resistor. Connect green and black to 0v and Blue to an input.
Take the 5v and 0v from your breakout board if it has connections for them.
You may need to widen the slot, it looks narrow, I used to use 10mm wide slot on a 100mm disc and it worked great. Also remember to make sure the Index Debounce is set to 0 in General Config. Some people have needed a small amount of Index debounce when using different sensors but with the OPB optos I always had it at zero.
Hood
-
oh ok
i dont have 5v to take from BOB so im using a seperate one of these -
http://www.ebay.co.uk/itm/220986283308?ssPageName=STRK:MEWAX:IT&_trksid=p3984.m1423.l2649
slight over kill i know but its all ive got at the moment
my slot is 4mm wide, to narrow? my disk is just 70mm dia
-
What make/model of BOB do you have?
If using a separate power supply then you will likely need to tie its 0V to a 0V on your breakout so that the signal is being referenced at the same potential .
4mm may be ok, try and see, you will soon know as when you spin fast you will not get an accurate reading if it is too small
Hood
-
ive no idea, ill phone angel tech later and double check with him, unless he replies here first.
-
all wired up i think?
just not sure on how to set up ports and pins.
i believe im connected to input 12. so i activated input 12.
but im getting no reading still
-
You set the Index input to the port and pin number you have it connected to.
Hood
-
hood, is this a slow sensor or something?
got a 11mm wide slot and the highest rpm reading i can get is 1340
my machine goes up to 4000rpm
cheers
-
Have you remembered to set Index Debounce to Zero?
The sensor is plenty fast so shouldnt be an issue with that, the BOB may be a problem, could have slow optos on it?
Hood
-
the sensor is connected straight to the db25 connector, not to the BOB
debounce is at 0
-
Shouldnt be a problem then, can you attach your xml and I will take a look to see if there is an issue in it.
Hood
-
errr sure but ive not got a clue what your talking about lol
what file and where do i find it?
also i keep snapping taps, im using this code
m3 s1000
g00 x20 y0
g00 z3
G95
G1 Z-10 F0.5
G1 Z5
G94
m5
m30
-
The xml is in the main Mach3 folder and will have the name of the profile you are using followed by a xml file extension. You will need to copy it to your desktop then rename to attach to the forum, call it andy_con.xml and that should work.
You need to have a short rapid retract for that tapper, if I recall correctly, to engage the reverse clutch quickly.
Hood
-
will pm you file
um short, could you tweak my code so i can see what you mean?
-
m3 s1000
g00 x20 y0
g00 z3
G95
G1 Z-10 F0.5
G0Z-2 <..........You will need to read the PDF that was attached earlier to see the distanbce required, I was thinking it was 8mm
G1 Z5
G94
m5
m30
-
ah right so a fast up then a slow retract
might have missed the pdf will go look
-
um yes it seems to say retract as fast as you can
Retract Tapping
head at 13,000 mm/
min or 500 in/min,
specified distance
for specific tapping
head to reverse tap
rotation.
-
You have a max speed of 1m/min so just do a G0 and that will assure its at the fastest speed you can do.
Hood
-
Are you still using the power supply to power the opto?
Try using your computers 5v and see if its better, you can grab the 5v from either a USB or a spare molex connector, if using the molex then 5v is red and black is 0v.
Hood
-
yes im using a proper bench psu at the moment to supply the 5v
-
Have you tied the 0V of the bench supply to the 0V of the parallel port?
Hood
-
nope, but guessing i should be
-
You may not get a correct signal if you dont as your bench supply may be at a different potential than your computers supply.
I would however think you would get erroneous signals at all speeds if that was the problem though.
Hood
-
will give it a try
-
WHen I made the disc for the BP here I used a 50% factor for the on off. THere ended up being half the disc cut away. It reads precisely as fast as the spindle will run 5000 rpm.
That was with using the LPT port driver.
(;-) TP
-
Mine used the OPB 917B opto and the disc was about 90mm OD with a 10mm slot and it worked fine up to, if I recall, 5000 as well. I usually never went above 4000 on the BP but I did test by cranking up the VFD.
On the lathe I think it was again a 10mm slot but only a 70mm OD disc, the lathes top speed was only 2000rpm however but again it worked well.
Hood
-
I have no intention of throwing a blanket over this whole discussion becasue it is educational in finding out how to hook up an RPM indicator. BUT:
If you look at the video from Tapmatic - and from my experience doing it manually - as long as you are only tapping a hole maybe no more than a half an inch deep or so, all you need to do is set the tap into the hole. The tap will screw itself into the hole and the spindle of the tapping head will automatically extend by itself as the tap screws in. When the tap reaches the bottom of the blind hole the head internals will slip until you get aroud to lifting up on the tapping head. Then it will go into reverse unscrewing the tap.
With that said I figure all you need to do is emulate the action you take when doing it by hand. I.E. do a G1 down to a depth enough to get the tap into the hole to get the thread started. Then perhaps feed down very slowly a very small amount just to waste some time until the thread is complete. Then retract the head again quickly to ensure the tap is above the work. The tapping head knows how to do the job for you. I don't think you need to down-feed at any particular rate to follow the tap. That only complicates things. (it may depend on the type of head you have - not sure but mine works as described).
BTW andy_con.
There is a tension adjustment on the tapping head that ensures it slips if the tap binds up in the hole (or when it runs into the bottom of a blind hole). If you have that set too tight that might explain why you broke so many taps.
Just my 2cents worth - sorry for the interruption - now back to the discussion.
Sage
-
The clutch is a safety NOT a means to run the taphead. UNTIL you apply downpressure you will not engage the clutch that drives it down AND until you apply UP pressure it will not reverse itself and retract the tap.
Ideally I always run a touch of overfeed to insure good pressure on the clutch. Same with retract do the initial retract to set the clutch at MAX speed (G00) then feedup the rest of the travel. The idea is to get the tap retracted and NOT have a lot of excess spring pressure at the point just before it clears the surface to prevent it springing up and tearing the last thread or so.
Being it is a floated design it is not really RPM sensitive as long as you are close to what you tell the machine it actually is. IF you are off a few rpm it is not a big deal to the taphead.
Tapmatic GIVES you the proper sequence to follow for CNC use.
Just a thought, (;-) TP
-
ok spindle feedback fully working. all i had to do was connect gnd to pin 25 of the parallel port.
but i have snapped 4 taps tonight :(
-
OK HOW it it snapping taps overfeed under feed overretract moving OFF center before it is done ? are you using a tapping cycle or remming cycle or hand coding it. Are you getting a pause from mach during the cycle? Are you bottoming the tap ?
Drill size to small ?
Wrong H factor for hole size ?
Not using proper tapping fluid for application?
Can you describe what takes place that snaps the tap?
(;-) TP
-
BR549:
You are exactly correct. I've only used my head a couple of times and as usual my memory did not serve me correctly.
Things happen so fast in the video I guess I was seeing whatever supported my memory.
Sorry for the interruption.
Sage
-
NOT a problem I HAVE used the clutches a time or two (;-). But you have to be careful of the settings as IF it slips too much then you end up at the top of the retract BEFORE the tap clears the hole and when you move off it snaps the tap.
Proper tap for the application also plays a big role. Spiral fluted, spiral point botton tap, rollform tap. ??????? thru hole blind hole ,shouldered hole, recessed hole.
Chips can be a BIG problem with small taps.
(;-) TP
-
http://www.youtube.com/watch?v=ZGMC55t-98E
how do they tap so fast and go from one hole straight to the other without any swarf on the tap??
-
IF you use the correct hole size for application and the correct tap type AND the correct tapping fluid there is little swarf to stick to the tap.
(;-) TP
-
Prolly a forming tap also. What material are you trying to tap?
-
Also, spiral fluted taps are the most fragile taps there are. If you have a deep hole (enough for the chips to pack into) a spiral point would be stronger. If your tapping softer metals, a forming tap would be the strongest.
-
aluminium and blind holes
-
If it were me, I would go with a thread forming tap. Stronger threads, stronger tap, and best of all, no chips. Keep in mind they require a different size hole than cutting taps. M2's and 3's are pretty small taps to start out with, on an inexperienced method. Again, if it were me, I would use a larger, more forgiving tap, until I got the hang of it and learned a few "in's and out's" of the tapping head. Might save some money both on taps, and anger management classes.
-
IF you are doing small blind holes then Spiral points are NOT the tap you want. They push the chips ahead of the tap. Use a std or bottom tap and the H factor you need for thread spec.
You are a brave soul learning with M2-3 taps (;-) BUT a thread is a thread by any name or size.
(;-) TP
-
ok well i got the tapping head working
http://www.youtube.com/watch?v=bBzbPQNuNFk&feature=share
but another question
for an m3 tap i use a feed rate of 0.5
i have a special m9x0.5 tap, although much larger do i still use a feed rate of 0.5?
-
Your feed, if using feed per rev, is whatever your pitch is, the Dia has no bearing on the feed.
Hood
-
ok now although i have the head working its not going very well, it keeps snapping taps left right and centre. so i got in contact with tapmatic for a little help and heres the response i got
i shoudl use a bore in bore out program of g85 not g95.
also feed rate should be 95-98% of the calculated feed rate from the rpm.
could i get some more coding help please ;)
not had a chance to pull my gcode sheet out yet and look at g85 and probably wont get a chance to till tomorrow evening
-
OK Ill ask one more time WHAT is causing the tap to snap? Is it bottoming out ? XY moving before it clears the top ?? , or what???
The G85 is a boring cycle. Z down then Z up at feedrate. It does not have the fast retract in the cycle.
IF you want to try it it is described in the MACH3 manual.
The G95(Ipr) is to make your life simpler. IF you want to hand calculate the feedrate then use G94 (FPM)
(;-) TP