Hello Guest it is January 17, 2022, 01:35:48 AM

Author Topic: Success! Mini Machining Center under Mach3 control - Video link  (Read 331537 times)

0 Members and 1 Guest are viewing this topic.

Offline BR549

*
  •  6,952 6,952
    • View Profile
Re: Success! Mini Machining Center under Mach3 control - Video link
« Reply #290 on: January 27, 2015, 09:39:17 PM »
Steve When Tapping do you prefer a { Feed per (unit)} feed OR {Feed per REV} feed ?

I prefer FPR as it is easiest to program AND you can SSO and the feedrate follows the RPM.

(;-) TP

Offline simpson36

*
  •  1,369 1,369
    • View Profile
Re: Success! Mini Machining Center under Mach3 control - Video link
« Reply #291 on: January 28, 2015, 05:24:10 AM »
Tapping preferences:

Based on comments thus far, it seems this wizard is MACH4 only? I was not aware MACH3 supported G84

That being said, my mill spindle is servo powered, so I use a custom macro for rigid tapping. The macro is a bit complex. It first gathers and saves certain settings, performs a software 'swapaxis' to 'C' axis, performs the tap action at a set speed and dwell and retract. Settings are then restored on exit to what they were on entry.

To 'jump' over obstacles, there is a retract parameter. The macro first compares the current Z with the retract and if they are exactly the same, it assumes the tap is at retract Z and does a rapid to zero before executing the tap action. With this macro all tapping begins at Z zero being the end of the tap at the top of the hole. This can be accomplished with a G52 if it is embedded in a larger G-code program. I tend to use it 'manually' most of the time.

With the exception of the retract mentioned above, all motion is incremental. This allows any arbitrary and precise tapping depth while maintaining the same starting azimuth. Which in turn allows more than one pass for deep threads in stringy or hard materials.  

Having G84 available changes the landscape and I would agree that FPR would be preferable. I would only use G84 if M19 was also working and could be executed prior to the G84 for reasons cited above.
« Last Edit: January 28, 2015, 05:27:15 AM by simpson36 »

Offline simpson36

*
  •  1,369 1,369
    • View Profile
Re: Success! Mini Machining Center under Mach3 control - Video link
« Reply #292 on: January 28, 2015, 05:33:33 AM »
4th axis tapping:

ANY time I can TAP or DIE CUT threads, I take that rout . . . did I mention ANY.

Tapping to a center hole and/or driving a chucked workpiece into a die holder is stupidly simple so I tend to just write the code 'on the fly' into the MDI, but I think it would make a nice addition to a wizard.

The calc is quite simple and the whole operation is one line of Gcode  . .  well, two if you count backing out.

That brings us to single point threading,  . . . the holy grail . . . . which I will comment on separately.

Offline simpson36

*
  •  1,369 1,369
    • View Profile
Re: Success! Mini Machining Center under Mach3 control - Video link
« Reply #293 on: January 28, 2015, 05:53:21 AM »
4th axis single point 'universal' threading:

This is the 800lb Gorilla, especially if you are trying to meet a spec. for thread fit. I have experimented and tried so many methods it's just ridiculous and while I have several successful 'universal' threading G-codes and Macros, including some that will cut any arbitrary tapered thread, the 'perfect' solution continues to evade.

I have tried the 'old school' 29 degree step down learned from crusty old machinists many, many moons ago. This works great for aluminum, but 'not so much' for stainless. Then 'quadrant' type cuts where the thread form is broken down into interconnected 'blocks' in the manner of an FEA mesh. 'Farming' or 'plowing' where successive vertical or horizontal rows are removed followed by a configurable number of 'spring passes'.

The two main positioning methods I have used are actual ID/OD or a 'surface start' at Z zero (or Y zero depending on where the tool is). I will provide, privately, some of the carcasses of these animals for you to dissect if you think it may be useful and of course, I am happy to discuss different methods, theories, or ideas on the best approach, but I do not have 'the' answer to this one.  :-[

It would be great to get some fresh ideas on how to skin this cat. A theory to work on. I can cut threads, no doubt, but I don't have that grin . . . you know what I mean.




 

Offline BR549

*
  •  6,952 6,952
    • View Profile
Re: Success! Mini Machining Center under Mach3 control - Video link
« Reply #294 on: January 28, 2015, 10:45:41 AM »
Mach does support G84 motions BUT it does not sync the Spindlle to the Zfeed. IT may be possible but i will not let that cat out of the bag.

A servo spindle can be refhome back to the index mark to set the Spindle to 0.000.

An M84 can be created to create a rigid tap function. It can have 3 outside param calls P,Q,R to set inside variables.  The sequence can be done as a SUB so it SHOULD be able to  simulate the G84 function quite easily.

Crusty OLD Machinist (;-) ???? I resemble that remark a great deal (;-).

I can shuffle some more room on the page so IF you get time send me what you have code wise for what you do. I will look it over and see what we can do with it. Top secret of course(;-)

Single point threading THE HOLY GRAIL.  IT all depends (;-),  we will just throw it all in the frying pan and see if we get fried fish.

(:-)TP





« Last Edit: January 28, 2015, 10:47:21 AM by BR549 »

Offline BR549

*
  •  6,952 6,952
    • View Profile
Re: Success! Mini Machining Center under Mach3 control - Video link
« Reply #295 on: January 28, 2015, 07:00:08 PM »
OK i made some room and have 10 extra function buttons available.

IF you can explain what axiss you use to do the internal external threads I will give it a go. Should not be that hard :D (famous last words).

A picture that shows a distant view that shows ALL of the machine would help.

(;-) TP
« Last Edit: January 28, 2015, 07:02:57 PM by BR549 »

Offline simpson36

*
  •  1,369 1,369
    • View Profile
Re: Success! Mini Machining Center under Mach3 control - Video link
« Reply #296 on: January 29, 2015, 05:29:42 AM »
OK i made some room and have 10 extra function buttons available.

IF you can explain what axiss you use to do the internal external threads I will give it a go. Should not be that hard :D (famous last words).

The tool can be held in the Z or Y axis. Threads can be cut from the top or bottom (Z axis) or front or back (Y axis).  Just what you wanted to hear . . LOL!

It sounds like unnecessary redundancy, but consider that cutting internal threads is best from a lubrication standpoint to have the cutter at the bottom where the oil collects, however, with a large diameter part, it can be difficult to reach the bottom with a cutting tool before the mill head contacts the top of the part with the tool bar on the 'far' side of the head. This arrangement is needed for long parts and puts the mill head above the part and the shorter tool overhang to cut the top of the hole becomes the determining factor for the setup.

Fortunately X remains X, so it is primarily a matter of exchanging Z for Y and positive for negative moves.


A picture that shows a distant view that shows ALL of the machine would help.

(;-) TP

As it happens, at this very moment I have an Ultra Spindle mounted for final turning and drilling the CamLoc flange, so I can get a lot of fresh photos showing exactly the setups you want.

 8)

Offline simpson36

*
  •  1,369 1,369
    • View Profile
Re: Success! Mini Machining Center under Mach3 control - Video link
« Reply #297 on: January 29, 2015, 06:02:18 AM »
Should not be that hard :D (famous last words).

That's what I thought . . . . may I suggest that you not test with aluminum, but with DOM tube. Picture perfect threads on aluminum are all too easy. Clean internal threads on DOM tubing will earn you a case of beer.

Also remember that real threads are not pointy. They loose (((P/2)/TAN(30))/8) in height by spec. Given that bit of threading trivia, an uber convenient addition to any internal threading wizard would be a calculator that provides the correct actual ID for a given thread.

Then, when you are finished with the threading code, you can add the boring code ahead of it for 'on-stop-shopping'.

And as any good 'Crusty Old Machinist' knows, taper the back of the bore and lift the last thread to prevent creating stress risers in the part.  ;)

Offline simpson36

*
  •  1,369 1,369
    • View Profile
Re: Success! Mini Machining Center under Mach3 control - Video link
« Reply #298 on: January 29, 2015, 06:36:35 AM »

Crusty OLD Machinist (;-) ???? I resemble that remark a great deal (;-).

(:-)TP


In addition to your machining experience, which is extensive, you also are a wizard at G-code, so I can think of no person better equipped to create a truly 'universal' threading program.

I prefer scripts to G-code because of access to better math, but I sent you a couple of my internal threading G-code programs as well as a G-code fragment specifically for calculating multiple passes in a specific way for specific materials. Hopefully there my be a morsel in there that will be helpful.

Now I am chomping at the bit to see what you come up with and test the whole system ( and I think system is the right word). Perhaps I can entice you somehow into expanding the system to take advantage of the InTurn™ Turning capability in prepping the part prior to the drilling/tapping operations.


Now, one more fish for your pan; provide the coordinated motion to bore and thread holes that are not in the center of the part. Example: simple flange with 4 tapped holes on a single BC. With NO horizontal spindle, this can be accomplished using a stationary cutting tool by coordinating AYZ motions to create an 'orbiting' motion in the part that will allow drilling/boring/tapping off center.

'Should not be that Hard' . .  is a phrase that I heard somewhere . . .  :)


Offline simpson36

*
  •  1,369 1,369
    • View Profile
Re: Success! Mini Machining Center under Mach3 control - Video link
« Reply #299 on: January 29, 2015, 06:47:54 AM »
A servo spindle can be refhome back to the index mark to set the Spindle to 0.000.

Yes, but is this part of G84? I was thinking that M19 should precede G84 in order to provide the functionality of my tapping macro . . unless I have the number wrong. M19 homes the spindle, is that correct?


An M84 can be created to create a rigid tap function. It can have 3 outside param calls P,Q,R to set inside variables.  The sequence can be done as a SUB so it SHOULD be able to  simulate the G84 function quite easily.

My macro is M9000 but it works via param passing with P being depth, Q being TPI and R being retract. I think I described the behavior in an earlier post. I'll take a peek and post it here if I am mistaken. Edit: yes response #291

If I stick the macro in G-code, it is typically arranged as a sub, so we are still on the same page with that . . .  amazing . .   :D