Announcement

Collapse
No announcement yet.

Tormach 1100 as a shaper?

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts

  • Mark Davis
    replied
    Update,
    I have two pieces of 4140 to make actions, along with a couple peices for the falling blocks. Purchased some sqaure 3/16 HSS and started grinding the recomended 4 different cutters.

    My shaper tool does not lock the spindle when the collet sucks it up against bearing housing. How to lock the spindle has been the subject of thought, but not much action yet.

    Double sided tape would be almost to easy, just fitting the flat surface between the cup and the bearing housing. But the thought of it working at first, then giving way about the time the cut is finished has me spooked.

    I'm more inclined to make a clamp on the top side of the spindle. The low speed chive for the drive belt looks like about the only thing to get clamp on.
    My Tormach has the tool carousel and air spindle release.


    Leave a comment:


  • Bob La Londe
    replied
    That's excellent. I'm looking forward to seeing your progress on that. Even a short video of your shaper attachment doing its thing would be really really cool.

    Leave a comment:


  • Mark Davis
    replied
    I joined ebay last week. Bought some steel.

    Had trouble getting ebay to accept my card, but did get the steel bought. No paypal for me.

    Chucked up a 4.25 round 3" long chunk of hot roll mystery steel, My guess is A-36.. Faced it. Drilled .375 1.5" deep and bored it out to .760. Cleaned up the out side.

    Turned it around and centered it up in the 4 jaw. Cleaned up the out side, faced it and in three steps drilled it to .75 to accommodate a longer, fatter, boring bar.
    Bored to 2.15" diameter 2.625 deep.

    It's still chucked up, still have bore about 3.35 diameter 1.75 deep.

    When finished, this will be spacer that seats on the on the head of the machine, keeps the spindle locked in place and saves the bearing from any pressure. I plan to bolt another piece to this, that will be grabbed by the collet on end; and attach a tool holder to the other end.

    Last edited by Mark Davis; 02-17-2020, 12:27 AM.

    Leave a comment:


  • RB211
    replied
    M102 very well could be Centroid specific

    Leave a comment:


  • Bob La Londe
    replied
    I was curious so I spent a few minutes. For Mach 3 M47 is to repeat program from first line.,
    https://machmotion.com/blog/knowledge-support-mcode

    On the Tormach PathPilot supported M codes page it does not show M47.
    https://www.tormach.com/supported-m-codes-reference/

    LinuxCNC (Tormach PathPilot is a LinuxCNC derivative) also does not appear to list M47.
    http://linuxcnc.org/docs/html/gcode/m-code.html

    M47 may or may not work on PathPilot or LinuxCNC, but I have had poor luck with undocumented commands in the past. Can't hurt to try I guess.

    Leave a comment:


  • Bob La Londe
    replied
    Originally posted by RB211 View Post
    Use G91
    use a G4p1
    Then a M102 to auto repeat. The G4P1 gives you a 1 second pause between cuts so you have time to hit a cycle stop button, because it will loop indefinitely with the M102 command.
    Use MDI to set G91, and make the first cut, then open the file below and run it. It will auto repeat.
    run it in a simulator first to verify it does what you want, so you don't crash. I'm still learning myself.


    G00 X.005 Y.003
    G01 Z-1F5
    G0X-.003 Y-.003
    G0Z1
    G4P1
    M102
    As near as I can tell M100 - M199 are user defined M-codes. For example some 3D printers use those including M102 for extruder commands. Perhaps Acorn has their own predefined M102 that repeats code? Lots of machine controllers have their own special features.

    Leave a comment:


  • RB211
    replied
    Use G91
    use a G4p1
    Then a M102 to auto repeat. The G4P1 gives you a 1 second pause between cuts so you have time to hit a cycle stop button, because it will loop indefinitely with the M102 command.
    Use MDI to set G91, and make the first cut, then open the file below and run it. It will auto repeat.
    run it in a simulator first to verify it does what you want, so you don't crash. I'm still learning myself.


    G00 X.005 Y.003
    G01 Z-1F5
    G0X-.003 Y-.003
    G0Z1
    G4P1
    M102
    Last edited by RB211; 01-19-2020, 10:20 AM.

    Leave a comment:


  • Bob La Londe
    replied
    Originally posted by sansbury View Post
    Are you running PathPilot? This is a perfect use case for macros.
    Could you give an example of how you would use a macro to do this? I'd love to learn something new.

    I use macros for tool changes and other things in Mach3, but I'm not sure how I would use one for iterative code. Well I could put all the iterative code in a macro and call the macro, but that's effectively the same thing. I run PathPilot on one of my five mills, but I don't get into the control side of it much. I just give it good code and it works.

    Leave a comment:


  • sansbury
    replied
    Are you running PathPilot? This is a perfect use case for macros.

    Leave a comment:


  • Bob La Londe
    replied
    Almost forgot. The main reason I popped back on. Squaring your cutter to your machine. Adjustable parrallel. I know you need to grind reliefs, but higher up ont he tool you can leave it flat and square. Use an adjustable parallel to your vise jaws as you lock the cutter or cutter holder in place.

    The other thing I thought of is if you want to creep upon it with the doors open (and your face shield on) you could program a pause between strokes.

    Leave a comment:


  • Bob La Londe
    replied
    Learning basic g-code really isn't that hard. I guess that was kind of my point. Sure I struggled with it when I first started CNC machining without any real CAM program. I didn't need to struggle. I just needed to read the documentation that was available, and apply it. I wrote some of my first commercial code by hand with a calculator and a text editor. Some things I do today I could not do without CAD/CAM, but they aren't the only tool available.

    There is no solution to CNC machining (or any kind of machining) that is the best for everything, just like there is no single hammer that does all hammer jobs better than any other hammer.



    Leave a comment:


  • Bob La Londe
    replied
    If it helps you could switch to absolute for Z moves and back to incremental for positioning for scraping, but I think it just adds a lot of unnecessary lines of code. In my Z example the actual Z(-z) Z(+z) values would be relative to your starting height to reach your desired depth. Do the simple math one time and keep the code short.
    Last edited by Bob La Londe; 01-17-2020, 11:57 AM.

    Leave a comment:


  • Mark Davis
    replied
    Your code would be a start, The -Z value needs some attention. I have not yet played in the incremental zone, sure simplifies a project like this.

    The original plan calls for scraping small semi circles proud of the square corner in the reciever.
    Thought I could do it with a small drill, if done at each layer as the end mill cuts it way down.

    The man who wrote the book spent many years as a tool and die maker, well above my skill level.

    He wanted anybody who has access to mill to be able to make their own single shot falling block.

    I think. he never thought a hobbyist would have a CNC mill.

    Leave a comment:


  • Bob La Londe
    replied
    Well, if you keep square corners on your block you still need to shape (broach) square corners on the hole. My thought was if you write the code you want you don't need a fancy shaper attachment. Just grind some clearance on a square lathe bit and go for it.

    You have to indicate in anyway, so you know the coordinates. Just manually write some simple code to move forward, scrape a couple thou, move back, retract, move forward a couple more thou and scrape again. A bunch of drilling operations in CAM might work, but it wouldn't be as clean as some code written for the purpose. Five lines of code per cycle. If you take the finish pass with a quarter inch endmill that only leaves a fillet of material 1/8 wide to scrape. I would recommend NOT trying to mill that deep with a long reach 1/8 end mill. It will likely chatter badly.

    So with a 1/8 wide corner fillet to remove that means about 63 cycles to remove the corner with a scraping routine if you think you can remove .002 per pass. You could probably take larger bites to start, but by the time you get into the corner you might not. I bet you could write the code to do that operation in 15 minutes or less in a text editor. You will probably spend more time checking it than doing it.

    G90 (Set Distance Mode Absolute)
    G00 X(x) Y(x) Z(z)

    G91 (Set distance mode incremental)

    G01 Z-1 F(f) (Plunge at feedrate)
    G00 X-.003 Y-.003 (Clearance to retract)
    G00 Z1 (Retract)

    G00 X.005 Y.003 (Step forward along X return to same position along Y)
    G01 Z-1 (Plunge at feed rate)
    G00 X-.003 Y-.003 (Clearance to retract)
    G00 Z1 (Retract)

    G00 X.005 Y.003
    G01 Z-1
    G00 X-.003 Y-.003
    G00 Z1

    Copy Paste Repeat

    G90 (Reset absolute distance mode)
    M30 (End program).

    Don't over think a brute force operation. Obviously substitute your own values. This code takes progressive X scrapes of .002 to the right from the location set at the start of the program.

    Double check me of course. I could have it all wrong. LOL. Air cutting something new is always a good idea.

    Leave a comment:


  • Mark Davis
    replied
    [QUOTE=Bob La Londe;. You have a CNC, let it do the work.QUOTE]

    How true.

    Am I crazy? I have a CNC, why not write a drilling program, remove a bunch of meat from the slot. run a mill around, Make a couple fly passes, clean up with a diamond lap?

    Leave a comment:

Working...
X