Spindle speeds and feedrate cap


Results 1 to 12 of 12

Thread: Spindle speeds and feedrate cap

  1. #1
    Registered HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default Spindle speeds and feedrate cap

    I just got ONEcncXP today.

    In my usual style, I usually just poke around with stuff and see if I can make it work. To me this indicates how intuitive a program is. I usually read the help later on.

    Verdict: you guys have really done an outstanding job of the post configuration setup. I run a Shadow controller, and this uses some of the most off-breed command language of all of them, and I think I have most of them set up already.

    I did check the help index to see if it made reference to this next issue, but didn't see any reference to spindle or speeds.

    Okay, now for a potential problem I would like to discuss: the material and tool lists are fine and dandy. But, I think that there should be a general parameter in NC setup that asks us for the maximum speed of the machine's spindle, and hopefully, a comparison could be incorporated so that if the machine is running flat out, that the maximum feedrate for a given tool in a given material, at this speed cap, would be automatically calculated and inserted in the program. This would be good for everyone.

    Now as a side issue, my Shadow controller does not use direct rpm commands, but rather runs on a percentage of Max rpm, thus all my speed range commands are from 0 to 100. Is there any way to handle this kind of a speed command issue, by converting from actual rpm (as calculated from your material tables) into percentage for output into the gcode? This converted output would only need to appear when the gcode is created, and not within the tool setup when creating gcode. I was hoping that maybe you could add this option in the general tab/decimal options/spindle speed. FYI, the Shadow spindle commands are whole numbers only, no decimal permitted.

    Now, back to exploring........

    Similar Threads:
    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  2. #2
    Registered HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    No one has any comments about this? Do all your machines have unlimited spindle rpm's available?

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  3. #3
    Moderator wms's Avatar
    Join Date
    Mar 2003
    Location
    United States
    Posts
    923
    Downloads
    0
    Uploads
    0

    Default

    Hu,
    That's right my machines will turn up to 100,000 rpm and balance is no problem.

    But seriously, I don't pay too much attention to what the cam system suggests for spindle speed and feeds.
    I found I always want to "tweek" them anyway.
    So when I'm going thru the tool path wizard I adjust the speed and feed to my liking.

    I know in a perfect world it would be nice to have the system output the perfect speed and feed.
    And if you get all the variables set up in the material sheet and tool sheet, it will output code based on those variables. But things like max spindle speed and the condition of the work piece and the way a person machines will "muddy" the water.

    As for the spindle code needing to be a percent of max spindle speed. That's a new one to me. All my machines want an actual speed with no decimal point.
    So I'm not any help here.

    I guess I'm so used to "tweeking" my programs after post,(especially at tool changes) that I don't know any better.

    We still have the problem of the "First" move to part at tool change where it always goes to xyz instead of xy at clearance then to z. (The safe way)

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  4. #4
    Registered HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    Originally posted by wms
    Hu,
    That's right my machines will turn up to 100,000 rpm and balance is no problem.

    But seriously, I don't pay too much attention to what the cam system suggests for spindle speed and feeds.
    I found I always want to "tweek" them anyway.
    So when I'm going thru the tool path wizard I adjust the speed and feed to my liking.
    Yes, I can do that and we would all have to tweak. But, I am sure the intention of the programmers is to have a starting speed and feed that is theoretically correct. I've got one mill that runs at 2500 max and another running at 6000 max, so I think the effort to cap the speed at those figures and then adjust the feed according to the speed cap would be worth making, if the feature is incorporated within software at all. It is this exact lack of precision that has forced you and I to become the tweakers that we are


    I know in a perfect world it would be nice to have the system output the perfect speed and feed.
    And if you get all the variables set up in the material sheet and tool sheet, it will output code based on those variables. But things like max spindle speed and the condition of the work piece and the way a person machines will "muddy" the water.

    As for the spindle code needing to be a percent of max spindle speed. That's a new one to me. All my machines want an actual speed with no decimal point.
    So I'm not any help here.

    I guess I'm so used to "tweeking" my programs after post,(especially at tool changes) that I don't know any better.

    We still have the problem of the "First" move to part at tool change where it always goes to xyz instead of xy at clearance then to z. (The safe way)
    You have this Z problem? Hmmm, I know what you are referring to, but I don't see it. In your NC setup "Tool format" do you have a
    G00 Z{CR}
    inserted after, let's say, when your spindle turns on?
    Here is a sample of the way my program would begin, including the first few lines of the toolpath.

    G40
    G75
    G80
    G90
    X-4. Y0. Z1. G92
    T2 (.375 INCH 3/8 CARBIDE BALL MILL)
    F18.4569
    S9228 M3
    T200
    /Z1. = (G00 Z{CR} in your NC setup Tool Format, /= G00 in Shadow)
    /X0.6064 /Y-0.0952 /Z1.
    /X0.6064 /Y-0.0952 /Z0.05
    F9.2284
    X0.6064 Y-0.0952 Z-0.1
    X0.6202 Y-0.0489 I0.3627 J0.0023

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  5. #5
    Moderator wms's Avatar
    Join Date
    Mar 2003
    Location
    United States
    Posts
    923
    Downloads
    0
    Uploads
    0

    Default

    HU,
    I was not disagreeing with you.
    It would be great to have the things you talk about.
    I'm as lazy as the the next guy and any thing to make my life easy I'm for.

    About the z problem, I need to dig into the setup and get it set up to do as you say. I need a G43 z.1 h(t) in there.
    This needs to be after the tool change and after the first move to position.(with no z movement)
    Just haven't spent the time to get it just right.
    I told you I was lazy.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  6. #6
    Registered HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    WMS, what kind of machine config are you using?

    For that line that you requested:
    G43 z.1 h(t)
    I believe this equals what I have to use for executing the tool offset in Shadow/Bandit which is simply:
    T2 = the tool changer command
    T200 = the tool offset executes.

    Anyways, there is a lot of functionality built into the NC setup, and it takes a bit of trial and error to understand how to use it.
    A few simple entries in the right place here = an entire script in bobcad.

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  7. #7
    Moderator wms's Avatar
    Join Date
    Mar 2003
    Location
    United States
    Posts
    923
    Downloads
    0
    Uploads
    0

    Default

    Hu,
    Using the HAAS cfg.
    Your right about the few line thing.
    I guess I'll put down the remote and fix my problem as you have "shamed" me into it.
    I also cleaned my PM up and cleaned my temp file now the Pm messages should be flying in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  8. #8
    Registered HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    Yes the new version fixes your decimal point in S parameter issue.

    From your Tool format for Haas:
    M5 G40 G49 G80
    M9
    ({TDES})
    {T} G43 {H} {D}
    M6
    {F} {S}
    M3
    {COOLANT}
    G0 Z{CR} <--- added this


    Got this for output. What do you think? You can try adjusting the Zero options before you post, too. That may have a favourable impact on your initial Z height. It seems to add on.

    N90 G0 G40 G49 G80
    N100 G0 G90 G54
    N110 M5 G40 G49 G80
    N120 M9
    N130 (.375 INCH 3/8 CARBIDE BALL MILL)
    N140 T2 G43 H2 D2
    N150 M6
    N160 F18.4569 S9228
    N170 M3
    N180 G0 Z1.
    N190 G0 X0.6202 Y-0.0488 Z1.
    N200 Z0.05
    N210 G1 Z-0.1 F9.2284
    N220 G3 X0.625 Y-0.0001 I-0.2468 J0.0488 F18.4569
    N230 X0.625 Y0.0001 I-0.125 J0.0001
    N240 X0.6202 Y0.0488 I-0.2516 J-0.0001

    Last edited by HuFlungDung; 04-05-2003 at 04:10 PM.
    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  9. #9
    Moderator wms's Avatar
    Join Date
    Mar 2003
    Location
    United States
    Posts
    923
    Downloads
    0
    Uploads
    0

    Default

    Hu,
    Thanks I'll give it a try.
    Sorry I was downloading that file we talked about.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  10. #10
    Moderator wms's Avatar
    Join Date
    Mar 2003
    Location
    United States
    Posts
    923
    Downloads
    0
    Uploads
    0

    Thumbs up Tool change

    Hu,
    This what I came up with.
    It's not exactly the way I want but real close.

    Start lines
    {T} M6 ({TDES})
    G90 G80 G40 G55
    {s} M3
    G43 {H} / M8


    End line

    M01


    Notes:
    {T} M6 ({TDES}) = Tool number, tool change, tool description
    G90 G80 G40 G55 = Reset canned cycles, set work offset
    {s} M3 = Spindle speed, turn spindle on clockwise
    G43 {H} / M8 = Set tool length offset, tool length number, block delete, coolant on

    Works for me but I would like a way to make the first xy move after tool changes (at tool changer height) with no z move, then turn on tool length and then move to a safe z clearance.


    The way it is now is if you put "Extra clearance" in the clearance plane, it will move there every time it goes to clearance.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  11. #11
    Registered HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    WMS,

    I was noticing the differences in the number of Z options offered in OnecncXP's drilling cycles, versus what you are offered in the mill pathing.

    I wonder why they cut those out? It seems that the extra clearance height in the drilling options is just what we need to be able to use everywhere, not just in drilling.

    What do you think? Compare the gcode output you get before a drill cycle with the output you get before milling.

    Maybe this would be worth petitioning for if you find it will fill the need.

    In my case, I used to use my controllers tool length offset option to serve as my "extra Z" option, ie., I would move to the start XY coordinate and then execute the offset, which my controller actually forces an immediate tool movement of the offset amount. This method is difficult to implement, too, because then I need to be able to insert that offset command after the first line of coordinate code has been generated. This is possible in the drill cycle setup, however, for regular milling, it is imperative to also have this tool offset command in the start line box, which in effect, give me two instances of the same command written into my gcode whenever I use a drill cycle.

    Last edited by HuFlungDung; 04-09-2003 at 08:50 AM.
    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  12. #12
    Registered
    Join Date
    Jun 2005
    Location
    Austria
    Posts
    93
    Downloads
    0
    Uploads
    0

    Default

    As a newbie, I would LOVE for a CAM application to ask me a few questions. Like: What spindle speed are you using? What type of material? You already include end mill size, so how about a little help on feed speeds? Great Idea, too bad I know very little about programing.



Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Spindle speeds and feedrate cap

Spindle speeds and feedrate cap

Spindle speeds and feedrate cap