Announcement

Collapse
No announcement yet.

Tormach 1100 as a shaper?

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

  • Tormach 1100 as a shaper?

    I just purchased Walter Mueller's book on building on building a single shot, falling block action.

    The book recommends using a shaper to make a finish cut for the slot the falling block rides in. Since most of us do not have a shaper, he designed and built a tool holder to fit a mill so it could be used as a shaper.

    The only mill I have is the tormach, and the thought of writing a bajillion lines of error free code is daunting. After a couple nights sleep on it, it occurred to that I could use CAM and drilling cycles to avoid errors.

    Anybody here ever do such a thing?

  • #2
    I imagine the Tormach would handle it just fine if you take a few thousandths per pass. It might be a good idea to setup a spindle brake or spindle lock of some kind. I'd be curious to know what your CAM approach would be.
    *** I always wanted a welding stinger that looked like the north end of a south bound chicken. Often my welds look like somebody pointed the wrong end of a chicken at the joint and squeezed until something came out. Might as well look the part.

    Comment


    • #3
      The tool is designed to press against the spindle bearing housing, when the collet closes. Locking it in place, and putting the cut pressure on the housing instead of the bearings.

      The book recommends .007 Doc and .003 traverse, That would be .007 X on the first cut, and .003 Y for successive cuts, the Z cutting stroke will be 2.25. I was considering a CAD drawing with .001 diameter holes, in rows .003 apart. Send it to CAM as a drill operation.

      An easy, cheap, safety would be remove the drive belt.

      But my reason for asking the question is hoping to get other ideas to consider. Since my budget is spent this month, next month I can order materials to make the tool, (3.5" Steel rounds just does not exist in my scrap pile) and some 4140 to make the receiver. Still have time to plan.
      Last edited by Mark Davis; 01-13-2020, 05:48 PM.

      Comment


      • #4
        Sounds like something you could make, and just use a square tool bit. You probably already have a few of those if you have a lathe.
        *** I always wanted a welding stinger that looked like the north end of a south bound chicken. Often my welds look like somebody pointed the wrong end of a chicken at the joint and squeezed until something came out. Might as well look the part.

        Comment


        • #5
          Yes, plan calls for 3/16 bit held in an extension made from .625 drill rod. The extension tool holder is 4.88 long, to fit in a socket on the shaper tool, make the 2.5" cut, the receiver sits at a 7.333 angle, plus hold the bit.

          The shaper tool has a toggle built in so on the back stroke the point of the bit will not drag.

          Comment


          • #6
            I like the Idea and plan to try it on my 1100 ...certain control would be there such as putting a little taper in the keyway which normally is hard to do. Now the machine reborn as a CNC vertical slotter

            Comment


            • #7
              A long time ago I wrote some macros for using Excel to create incremental G-Code. I think this would be a perfect application for that. You could just put it in your code to step back before retracting. It would allow for a simpler easier to make bit holder. You have a CNC, let it do the work.

              Excel did the incremental math bits, and the macros read the values as text and created the g-code. Then I just cut and pasted it to a text editor for any additional code tweaks.
              *** I always wanted a welding stinger that looked like the north end of a south bound chicken. Often my welds look like somebody pointed the wrong end of a chicken at the joint and squeezed until something came out. Might as well look the part.

              Comment


              • #8
                [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?

                Comment


                • #9
                  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.
                  *** I always wanted a welding stinger that looked like the north end of a south bound chicken. Often my welds look like somebody pointed the wrong end of a chicken at the joint and squeezed until something came out. Might as well look the part.

                  Comment


                  • #10
                    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.

                    Comment


                    • #11
                      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, 12:57 PM.
                      *** I always wanted a welding stinger that looked like the north end of a south bound chicken. Often my welds look like somebody pointed the wrong end of a chicken at the joint and squeezed until something came out. Might as well look the part.

                      Comment


                      • #12
                        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.



                        *** I always wanted a welding stinger that looked like the north end of a south bound chicken. Often my welds look like somebody pointed the wrong end of a chicken at the joint and squeezed until something came out. Might as well look the part.

                        Comment


                        • #13
                          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.
                          *** I always wanted a welding stinger that looked like the north end of a south bound chicken. Often my welds look like somebody pointed the wrong end of a chicken at the joint and squeezed until something came out. Might as well look the part.

                          Comment


                          • #14
                            Are you running PathPilot? This is a perfect use case for macros.

                            Comment


                            • #15
                              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.

                              *** I always wanted a welding stinger that looked like the north end of a south bound chicken. Often my welds look like somebody pointed the wrong end of a chicken at the joint and squeezed until something came out. Might as well look the part.

                              Comment

                              Working...
                              X