• Spring 2024 meetup in Calgary - tentative date Saturday, April 20/2024. Other regions are also discussing meet ups. If you want one in your area get going on organizing it! discussion
  • We are having email/registration problems again. Diagnosis is underway. New users sorry if you are having trouble getting registered. We are exploring different options to get registered. Contact the forum via another member or on facebook if you're stuck. Update -> we think it is fixed. Let us know if not.
  • Spring meet up in Ontario, Newmarket, April 6/2024. Discussion

HAAS CNC manual milling (fly by wire milling)

Janger

(John)
Administrator
Vendor
I was googling and googling on how to use the HAAS CNC Mill to manually mill something. ie use the MPG hand wheel to move an axis back and forth to just do some silly little thing like true up the end of stock or drill 1 hole. I want to do this because to use the mill I know of 3 ways to operate it yet they are all slow to setup. I just could not find anything relevant on how to operate the machine without writing or generating gcode, and I finally figured it out last night while discussing it with Dabbler. This is how CNC is less productive than manual machining for small jobs. Normally you have to generate that GCODE somehow. Here are the three (now 4) main ways I know of to operate the machine:

1. Manually write GCode by hand. Yes you can do this but it's easy to make mistakes and for heaven's sakes HAAS why can't I plug in a normal keyboard? There is a USB port! I touch type so a normal keyboard is miles faster. Any hand written keyboard gcode needs to be verified - carefully and suspiciously examined as it runs. Don't crash! You probably should to do a dry run above the part. So it's slow to use. It is just like writing & debugging a software program but there is no UNDO and bugs could result in real life crashes.

2. Use the HAAS CNC built in wizards to generate GCode. I do this and it's quicker than writing gcode by hand usually but still there are often 10 or 20 parameters to think about and set. It's easy to to get one wrong and you still need to carefully execute the program. Some things you think should be easy are missing from the wizards. Like a simple side milling wizard (curious oversight).

3. CAD/CAM. Design the part in Fusion 360, switch to CAM mode, build the stock model and then setup all the required milling tooling & operations, Simulate the job to look for problems. Then generate the gcode file and move it to the machine over wifi. With method 3 it is an hour at least for me anyway. Probably a day on a harder part and then a bunch of rework while I get the bugs out and repost. It's the fastest way to make a second part or 1+X number of parts but the first part is slow to produce.

4. Use the jog mode and manually move the table and spindle using the MPG wheel. Trouble I've been having is turning on the spindle while in JOG mode. It seems I need one line of gcode to get it started. The code turn on and set the spindle RPM:

M03 S1200; <- turn on the spindle to 1200rpm

Here I am assuming there is a tool in the spindle, the coordinate system is set (say G54), and all other modal commands are off.

This program turns on the spindle. To use put it in single step mode, press cycle start and the spindle turns on. Now you can use JOG to move the axis AND start the spindle with the FWD STOP REV buttons. (The doors have to be shut). Without the GCode M03 S1200 the spindle won't turn on - I guess because the machine does not know what speed to run the spindle. So this could be handy for example to square up some stock or drill a hole. Like on a manual mill I have to turn the MPG wheel through all the required operations so there is no walking away while the mill works. But hey no programming and there is DRO read out for positioning. :cool:

Anybody else using manual operations like this to manually make parts on their CNC? And does anyone else have another way than these 4?
 
Last edited:

Dan Dubeau

Ultra Member
I run a variety of haas mills at my day job (vf2, 3, 5, 6). And use them quite a bit as manual machines, Using only the jog wheel (and jog lock with feed override for power feed) to move them. Mostly for stock squaring/sizing operations. There simply is no comparison to a bridgeport style mill once you get used to it, and utilize it capabilities. Not even close. Preset tooling at the press of a button, and much higher horsepower and rigidity. Flood coolant, and full enclosure are just the icing on the cake too. Running a 5" face mill taking off 0.2" in one pass to bring a block to size.....no problem :D. There is no need to finger cam simple moves like facing operations etc. But you can have some easily editable ones in the control if you'd like. I used to do that, but barely use them anymore. The MPG wheel is great. If it's a detachable hand control even better. The stock placement leads to shoulder issues......

I almost never program at the control, and my MDI screen has "T## M06 S2500" about 99% of the time. I MDI T6 (or whatever tool #) "alter" to change tools, but you can simply do it by also typing T6 "Toolchanger fwd/back" as well. To run the spindle in hand jog mode you need to call a spindle speed like you mentioned, otherwise it has no modal command for spindle speed set, and the CCW/CW buttons do nothing. I will occasionally change my S2500 to higher, but I've found 2500 is a good compromise to override up/down for the tools I typically run manually. Anything else I'm quick in cam, and just do it that way.

Just a side note. When I turn the machines on, I ALWAYS run a warmup spindle program before machining (and after dissabling the door lock...:)). There is always one supplied with every HAAS from the factory, and if yours doesn't have one someone probably over wrote it. Spindle speed is a modal M command which means once called it's always active unless uncalled, or changed. So running the warmup solves the problem of calling a spindle speed command by having it set by the program. I've changed the last line of my warmup programm on all the machines to reset the speed back to 2500rpm, to maintain continuity. I like working a specific way.......
 

Janger

(John)
Administrator
Vendor
5" face mill at 0.2" DOC? Holy hoggin batman. :cool::cool::cool:

I appreciate the notes on how you operate Dan. What CAM are you using? Do your machines use WIFI or do you sneaker net around with USB Drives? Or RS232:)p)

I do use the wizards on my new generation control but I don't know that older machines have those wizards? Below are the wizards available. And also the buttons for spindle control. I guess you don't use or can't use wizards since you didn't mention it.
 

Attachments

  • BFD38139-F0AE-4DF5-BCAB-8FD536FC3535.jpeg
    BFD38139-F0AE-4DF5-BCAB-8FD536FC3535.jpeg
    372.5 KB · Views: 6
  • 362E6DFA-BE35-4266-BA32-3DC0CC44459B.jpeg
    362E6DFA-BE35-4266-BA32-3DC0CC44459B.jpeg
    258 KB · Views: 6
Last edited:

Dan Dubeau

Ultra Member
The 5" face mill is an iscar high AluMill. It's a beast, and will go deeper..... We also have a 2.5" one, and a few 1"/2" seco versions of the same style cutters. Most brands have similar lines though, similar shape to an apkt insert but aluminum specific, and all proprietary. They are amazing for material removal, and leave amazing surface finishes too for both shouldering and faceing. Very low tool pressure so they make machines like a HAAS look like amazing. Inserts are expensive though, but last a very long time. You can easily fill a few 55gal drums with chips of6061 off one edge.

I use Edgecam, and sometimes MADCam (rhino plugin). All the machines except the vf5 are run via drip fed rs232 connections from old computers next to the machines. The vf5 is usb. I wish they were all wifi connected, but they are various vintages going back to mid 90's early 2000's. The USB machine is closest to my office, and the one I run the most so I'm used to it. If it was in the back corner where the vf3 is, I'd probably hate it lol. It is WAY more reliable running long finishing programs over night compared to the rs232.

None of them have quick code either (what is now called wizards I guess?), or I would probably use it a bit more. I have never in my travels seen, or run a machine with quick code, so I guess it wasn't a popular option for machines around here, but have read about it over on PM. I have conversational on my Tormach at home, and have grown to like it for quick operations. Took a bit of forcing myself to use it, as I'm pretty quick with CAM, but it is nice sometimes just to do stuff right at the control. Dollars to doughnuts I think it would be a toss up as to what I'm quicker with. Depends on what I'm doing with it I guess.

What machine do you have?
 

Chipper5783

Well-Known Member
A few simple lines of G1 is no big deal. Of course if you goof up the numbers, you’ll get a bad outcome - same problem on a manual machine. I pump in manual Gcode all the time (either at the machine or with a simple text editor). For a quick cut, I’ll often go to the VMC, for all the reasons that Dan pointed out (I have 3 decent manual machines, they mainly get used when I don’t want to disturb a set on the VMC).

My VMC is an old Bridgeport product, if anything major bad happens to it - then it becomes a boat anchor. I have fixed a number of small issues and it is working well, but I fear that one day some smoke will come out and it will be cost prohibitive to repair (depends on what that someday future problem is). I’m steadily moving to the point where I’d be pretty lost without it - but to replace it with equivalent capability is a lot of $$.
 

Janger

(John)
Administrator
Vendor
The 5" face mill is an iscar high AluMill. It's a beast, and will go deeper..... We also have a 2.5" one, and a few 1"/2" seco versions of the same style cutters. Most brands have similar lines though, similar shape to an apkt insert but aluminum specific, and all proprietary. They are amazing for material removal, and leave amazing surface finishes too for both shouldering and faceing. Very low tool pressure so they make machines like a HAAS look like amazing. Inserts are expensive though, but last a very long time. You can easily fill a few 55gal drums with chips of6061 off one edge.

I use Edgecam, and sometimes MADCam (rhino plugin). All the machines except the vf5 are run via drip fed rs232 connections from old computers next to the machines. The vf5 is usb. I wish they were all wifi connected, but they are various vintages going back to mid 90's early 2000's. The USB machine is closest to my office, and the one I run the most so I'm used to it. If it was in the back corner where the vf3 is, I'd probably hate it lol. It is WAY more reliable running long finishing programs over night compared to the rs232.

None of them have quick code either (what is now called wizards I guess?), or I would probably use it a bit more. I have never in my travels seen, or run a machine with quick code, so I guess it wasn't a popular option for machines around here, but have read about it over on PM. I have conversational on my Tormach at home, and have grown to like it for quick operations. Took a bit of forcing myself to use it, as I'm pretty quick with CAM, but it is nice sometimes just to do stuff right at the control. Dollars to doughnuts I think it would be a toss up as to what I'm quicker with. Depends on what I'm doing with it I guess.

What machine do you have?
I have a HAAS TM-1P. I have some facing cutters with the APKT inserts - the aluminium specific ones are sharp and do work well. I would not have tried hogging like you do, perhaps if my machine was more rigid. For heavy hogging though I have a 2" face mill which uses those octogonal inserts. The inserts have 8 surfaces on two sides so potentially they go a long time. Do you use those Dan?

Can you get a RS232 to USB box to make those older machines easier to use? I know Alex got a floppy drive to USB box he put on his machine so he does not have to use floppies.
 

Janger

(John)
Administrator
Vendor
A few simple lines of G1 is no big deal. Of course if you goof up the numbers, you’ll get a bad outcome - same problem on a manual machine. I pump in manual Gcode all the time (either at the machine or with a simple text editor). For a quick cut, I’ll often go to the VMC, for all the reasons that Dan pointed out (I have 3 decent manual machines, they mainly get used when I don’t want to disturb a set on the VMC).

My VMC is an old Bridgeport product, if anything major bad happens to it - then it becomes a boat anchor. I have fixed a number of small issues and it is working well, but I fear that one day some smoke will come out and it will be cost prohibitive to repair (depends on what that someday future problem is). I’m steadily moving to the point where I’d be pretty lost without it - but to replace it with equivalent capability is a lot of $$.
What era Chipper is your bridgeport? Green CRT?
 

Janger

(John)
Administrator
Vendor
I have a TM-1P also (With 4th axis I’ve never used yet.)
Yah I checked out Tom's machine when I was trying to figure out what to buy. I decided the big work envelope was more important than the higher feeds on the HAAS Mini Mill. I really like my machine but I do wish the tool changer was double or triple in size.
 

Dan Dubeau

Ultra Member
I have a HAAS TM-1P. I have some facing cutters with the APKT inserts - the aluminium specific ones are sharp and do work well. I would not have tried hogging like you do, perhaps if my machine was more rigid. For heavy hogging though I have a 2" face mill which uses those octogonal inserts. The inserts have 8 surfaces on two sides so potentially they go a long time. Do you use those Dan?

Can you get a RS232 to USB box to make those older machines easier to use? I know Alex got a floppy drive to USB box he put on his machine so he does not have to use floppies.
I have not tried octagonal inserts, although I almost bought a 4" Seco Octomill a few years ago to replace our older facemill. The shop next door uses them, and loves them. Even though the TM is lighter construction than the VF's, you should still be able to take a decent chunk with the APKT aluminum inserts. They're pretty free cutting. I made a 1" TTS apkt holder for my Tormach, and it does pretty good with it, although I've never pushed it too much yet.

There are options to replace the rs232, but they all cost money. Some of them cost a few hundred which is too much for our little shop to spend on keeping the things that make us money going.......We have a mix of trusy old xp towers and one with 2000 on it, that are holding us together.....With a couple spares on the shelf. Rock solid :D.

Yah I checked out Tom's machine when I was trying to figure out what to buy. I decided the big work envelope was more important than the higher feeds on the HAAS Mini Mill. I really like my machine but I do wish the tool changer was double or triple in size.

That's my one gripe about our VF5 is the 20 pocket umbrella changer. I don't like umbrellas to begin with, but 20 tools on a machine that size sucks. Doesn't take long to fill it up with drills/reamers on some of my jobs. Will the TM allow you to manually change using alternate H#'s for extra tools? For example leaving an open pocket, and calling T10, H14 etc, and hand loading extra tools during a cycle?
 

Janger

(John)
Administrator
Vendor
I have not tried octagonal inserts, although I almost bought a 4" Seco Octomill a few years ago to replace our older facemill. The shop next door uses them, and loves them. Even though the TM is lighter construction than the VF's, you should still be able to take a decent chunk with the APKT aluminum inserts. They're pretty free cutting. I made a 1" TTS apkt holder for my Tormach, and it does pretty good with it, although I've never pushed it too much yet.

There are options to replace the rs232, but they all cost money. Some of them cost a few hundred which is too much for our little shop to spend on keeping the things that make us money going.......We have a mix of trusy old xp towers and one with 2000 on it, that are holding us together.....With a couple spares on the shelf. Rock solid :D.



That's my one gripe about our VF5 is the 20 pocket umbrella changer. I don't like umbrellas to begin with, but 20 tools on a machine that size sucks. Doesn't take long to fill it up with drills/reamers on some of my jobs. Will the TM allow you to manually change using alternate H#'s for extra tools? For example leaving an open pocket, and calling T10, H14 etc, and hand loading extra tools during a cycle?

Yes the TM-1 will support different tool and H offsets. I’ve not tried it yet. Another good thing to try. How do you keep track of which H index works with which tool? I’ve seen felt sharpie used to write on the tool holder and attempts at using labeler printed tags. I was thinking maybe engrave the index right on the holder.
 
Manual milling on a CNC piece of cake as long as you have a rotary dial. Treat it like a manual with DRO.

Don't know the HASS system personally, but on Centriod (Acorn) you can download a demo which contains Intercon which allows you to write Conversational code to write g-code. Your pic, as a 2d dxf would turn into g-code in less than 10mins. I'm now doing about 5000lines of g-code from 30 lines conversational with DXF and final tweaking in gwizard to optimize. In less than 20mins.

To mill a quick slot, touch off (as you would with any mill, and go at it with the the rotary jog. 0mins. Forget offset, and tooling just treat it as a manual mill,

Think CNC is an extension of manual and manual is an extension of CNC, don't over think it.

Just remember g & m codes are like language and have different dialects for different machines and cause slightly different results.
 
Last edited:

jcdammeyer

John
Premium Member
I use the MDI line on AXIS LinuxCNC for a lot of things.

And similar to Dan, I tool change with T## M6 G43 and have done an S1000 M3 at some point. After that the spindle ON/OFF button on the pendant or the screen start/stop the spindle at the last set speed.

Either the keyboard or the MPG is used for traversing. I agree there are a number of GCode commands to remember. But for cleaning up an edge it's usually easier to tell it G01 X2.0 F20 and then when it's done jog Y in a bit using the MPG and then since it remembers G01 just X0 to go back and mill again.

Or move Y so the cutter clears the work. G0 X0. Then move, with the MPG to the new cutting depth. G01 X2.0

And when done either the M5 to turn off the spindle, the button on the screen to turn off the spindle or the button the Pendant. Whatever is handy.

The MDI screen has a long history list so I normally just scroll up, select and enter to rerun a similar line.

The habit I haven't undone yet is reaching with my left hand to the old spindle ON/OFF switch. Really should wire that switch in to the tool changer module to generate the M3/M5. Project #42.
 

Chipper5783

Well-Known Member
What era Chipper is your bridgeport? Green CRT?
BP VMC was made in 1998. VGH monitor. Basically the HMI (human machine interface) runs on a pentium PC - Dos 6.22, it even has a 3.5” floppy drive (since converted to a USB mimic of a floppy). The advice I’ve been given is that if it works as original, then leave it alone. At the beginning there was a bunch of small things to fix, but the last ~3 years it has been working well for me. Looking at the conversion projects folks do, I have way less time and money than many people have in their manual to CNC conversions - and I’ve got flood coolant, full enclosure, 4 axis, chip conveyor, 22T changer, #40 taper and decent size work envelope. If something major fails, then it may all be scrap - so far I am thrilled with it.
 

Dan Dubeau

Ultra Member
Yes the TM-1 will support different tool and H offsets. I’ve not tried it yet. Another good thing to try. How do you keep track of which H index works with which tool? I’ve seen felt sharpie used to write on the tool holder and attempts at using labeler printed tags. I was thinking maybe engrave the index right on the holder.
If you find a good solution let me know.....

I have seen tags that snap into the v flange, and have seen people use paint pens to marked holders as well. The PO of my Tormach numbered all the holders with paint pens. But I don't use them that way, and think it's ugly (but that's not why I don't use it lol). I touch off whatever tools I need at the time for every job. I don't find it takes too long, and I'm alright with that for now. Simply engraving/etching a # into each holder and keeping a spreadsheet of the corresponding H# and offset would be pretty easy as a one man shop. Input that into your CAM tool table and you don't have to remember it.

About 10 years ago I came up with a system at work for all the standard bushing drills and reamers we shared amongst machines. They were all standardized, and never left their holders unless immediately replaced with new or resharpened. I used to have them all preset off the table of each machine and stored as higher H values, and kept track of them with a spreadsheet for TLO, and my tool table in edgecam to automatically post the correct H#. At the time we only had 2 machines (and 2 guys), and it was easy to reset all the tooltables based on the spreadsheet values if you needed to sharpen a drill, or change a tool. Just touch it off in whatever machine is open, and enter it in the spreadsheet to find the offsets for the other machines, then go change the values in the tooltables on each machine. Keeping track of what tools were what was simple, as they live in their holders and were easy to identify (a 3/4" reamer is easy to tell from 5/8" etc), the only tricky ones were the short stubby carbide drills for dowel drilling. I have metric, and Inch, and used black er nuts for the metric drills, and bright finish for Inch. It's easy to tell by eye which is which for all the drills and reamers as they are all stored in sequence in trays/carts. After a few times you can tell them all by eye.

We don't use that system anymore though. As we added more guys and machines, some of the new guys could not be trusted to retouch off tools and maintain the system after sharpening or replacing tools, so I decided to just scrapped it altogether. It was carnage for a while.......We still maintain the shared tools themselves, but the offset standard system is gone. The new guy I have now is pretty good, It's now just the two of us, so as he gets more comfortable with programming I've been trying to nudge him back towards that system as he's pretty good and reliable, but he's still pretty timid and not 100% confident in all the offsets and what they do.....I'm working on him.... Waiting for that ah ha moment. Touching off tools isn't that big of a process for the work we do, but it WAS nice to be able to just load tools and go......
 

Janger

(John)
Administrator
Vendor
BP VMC was made in 1998. VGH monitor. Basically the HMI (human machine interface) runs on a pentium PC - Dos 6.22, it even has a 3.5” floppy drive (since converted to a USB mimic of a floppy). The advice I’ve been given is that if it works as original, then leave it alone. At the beginning there was a bunch of small things to fix, but the last ~3 years it has been working well for me. Looking at the conversion projects folks do, I have way less time and money than many people have in their manual to CNC conversions - and I’ve got flood coolant, full enclosure, 4 axis, chip conveyor, 22T changer, #40 taper and decent size work envelope. If something major fails, then it may all be scrap - so far I am thrilled with it.
Nice features.
 
Top