Programming multiple parts per fixture - Page 2
Close
Login to Your Account
Page 2 of 2 FirstFirst 12
Results 21 to 38 of 38
  1. #21
    Join Date
    Jan 2013
    Location
    Gilbert, AZ
    Posts
    5,874
    Post Thanks / Like
    Likes (Given)
    7400
    Likes (Received)
    7464

    Default

    It is too bad autodesk is ruining FeatureCAM. It has the best multiple fixture function I have seen in any CAM system.
    I have not seen everything. But, I use the hell out of FeatureCAM's "multiple fixture document".

  2. #22
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,311
    Post Thanks / Like
    Likes (Given)
    747
    Likes (Received)
    1795

    Default

    Quote Originally Posted by Jmaks View Post
    Keep in mind the amount of tool changes with some of these suggestions.
    Fusion let's me order by tool change, and on the Fadal that's possibly the biggest time saver of all.

    Sent from my SM-G973U using Tapatalk

  3. #23
    Join Date
    Mar 2016
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    336
    Post Thanks / Like
    Likes (Given)
    74
    Likes (Received)
    186

    Default

    Quote Originally Posted by Cole2534 View Post
    Fusion let's me order by tool change, and on the Fadal that's possibly the biggest time saver of all.

    Sent from my SM-G973U using Tapatalk
    The biggest time savor for me is sequencing your toolpath along with limiting tool changes. Depending on the type of parts you are making I find that if I can eliminate a lot of lead in and lead out moves along with those rapid to clearance moved over to the next part is a huge time savor. Sometimes this requires me to chain toolpath together on multiple parts to really see the time savings.

  4. #24
    Join Date
    Aug 2008
    Location
    Philadelphia,PA
    Posts
    125
    Post Thanks / Like
    Likes (Given)
    17
    Likes (Received)
    10

    Default

    Quote Originally Posted by Cole2534 View Post
    Fusion let's me order by tool change, and on the Fadal that's possibly the biggest time saver of all.

    Sent from my SM-G973U using Tapatalk
    But when you use subroutines with fusion it writes a new program (even though it is the same program) for every single offset when doing order by tool. That is the dumbest thing I have ever seen. It requires an incredible amount of hand editing to remove the extra programs.

  5. #25
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    1,712
    Post Thanks / Like
    Likes (Given)
    157
    Likes (Received)
    200

    Default

    Quote Originally Posted by EnginCycles View Post
    But when you use subroutines with fusion it writes a new program (even though it is the same program) for every single offset when doing order by tool. That is the dumbest thing I have ever seen. It requires an incredible amount of hand editing to remove the extra programs.
    Have you contacted AD's post group to see if they can modify the post you are using to not add the extra programs?

  6. #26
    Join Date
    Aug 2008
    Location
    Philadelphia,PA
    Posts
    125
    Post Thanks / Like
    Likes (Given)
    17
    Likes (Received)
    10

    Default

    Quote Originally Posted by len_1962 View Post
    Have you contacted AD's post group to see if they can modify the post you are using to not add the extra programs?
    I did a few years ago and they said it was something they knew was an issue. Well here we are about 1000 updates later and it still seems to be the same. I don't think it would be a post issue and more of the actual program thing. I use multiple machines with different post's so I would prefer it is corrected within the program.

  7. #27
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    626
    Post Thanks / Like
    Likes (Given)
    84
    Likes (Received)
    303

    Default

    I am 99% there is a magic check box in Fusion 360 for that now because I ran into your issue a few months back. I can't for the life of me find it now but it wasn't just the check box in the post-processor popup. Maybe it was the "override WCS" box in the setup edit screen?

  8. #28
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,311
    Post Thanks / Like
    Likes (Given)
    747
    Likes (Received)
    1795

    Default

    Quote Originally Posted by EnginCycles View Post
    But when you use subroutines with fusion it writes a new program (even though it is the same program) for every single offset when doing order by tool. That is the dumbest thing I have ever seen. It requires an incredible amount of hand editing to remove the extra programs.
    I wish I was smart-enough to use subs. I'm still pretty wet behind the ears.

  9. #29
    Join Date
    Aug 2008
    Location
    Philadelphia,PA
    Posts
    125
    Post Thanks / Like
    Likes (Given)
    17
    Likes (Received)
    10

    Default

    Quote Originally Posted by Rick Finsta View Post
    I am 99% there is a magic check box in Fusion 360 for that now because I ran into your issue a few months back. I can't for the life of me find it now but it wasn't just the check box in the post-processor popup. Maybe it was the "override WCS" box in the setup edit screen?
    I am not aware of a box that says that. I looked in every single place I can think of and it is not there. Multiple WCS offsets is what I use but again it makes a new program for every instance of the same program. To dumb it down if you have a 1/4" hole drilled in the center of part it will write the code for that subroutine as many times as you are making parts. Instead it only needs to write the program once. Correct me if I am wrong but is that not the point of using M99/M98!

  10. #30
    Join Date
    Jun 2006
    Country
    UNITED STATES
    State/Province
    Alabama
    Posts
    1,876
    Post Thanks / Like
    Likes (Given)
    1088
    Likes (Received)
    736

    Default

    The best most fool proof way I've found is to "transform" each op using different Work offsets. Say you're spotting holes on three different parts, each one will have a G54, G55, G56 and run that spot tool, basically same program, just a diff offset.
    Most CAM programs will automate this easily.
    Doing it this way will minimize tool changes as it will say spot, drill, then Tap all parts in succession

  11. #31
    Join Date
    Aug 2008
    Location
    Philadelphia,PA
    Posts
    125
    Post Thanks / Like
    Likes (Given)
    17
    Likes (Received)
    10

    Default

    Quote Originally Posted by Rstewart View Post
    The best most fool proof way I've found is to "transform" each op using different Work offsets. Say you're spotting holes on three different parts, each one will have a G54, G55, G56 and run that spot tool, basically same program, just a diff offset.
    Most CAM programs will automate this easily.
    Doing it this way will minimize tool changes as it will say spot, drill, then Tap all parts in succession
    Not sure if you have Fusion but it does that already. If you order by tool it will do the spot drill at all the work offsets (say G54.1 p1,p2,p3). The issue is it clogs the menu up with 4 programs there when it could be 2 programs. Now add a part that has 12 steps and has 8 offsets. That adds 88 unwanted programs which is totally stupid.

  12. #32
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    272
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    86

    Default

    Not here to get into an argument about the virtues of full on CAM to post processor program generation compared to CAM aided manual programming, but in reading through this post and seeing the fretting and trials and tribulations of those so deeply stuck in and/or reliant on CAM and posts, really makes me glad to have the ability to program manually. The crux of this thread is something very elementary to programming, but it appears many people struggle just to find the right buttons to push inside CAM, (if they even exists as it appears) when all that is needed can be simply typed out, then copy and pasted to no end while covering the functions and progressions of countless tools used to create single or multiple work pieces.

    Below is a sample copy of what a multiple work offset program using subs should look like. (Fanuc) This sample represents 5 twin station vises making ten separate parts on a machine with additional work offsets available. (G54.1Type) If you do not have extra offsets, there are on-the-fly work offset methods you can create using G10 stuff that I'm not going to get into here. The offsets in succession represent the forward vise stations going left to right, then to the rear and heading back right to left. Meaning a CCW circle around the vise stations with each tool. This regime keeps the axis movement between tools to nearly zero. The block skips, when used, will produce parts in the first or left most vise only. I use the block skip for proofing the programming, and/or when running out the last few odd pieces of stock left over in a run.

    If your post is punching out stuff that looks completely different then shown below, then your post has problems. Realize the subs being called can be the most elaborate and amazing tool paths CAM software can come up with, but the basic master program can be typed up in minutes, and then repeated with good ole copy and paste. Truth be told, this could be made even shorter by combining the work offset and subroutine calls on the same line, but I like it like this for clarity, and it gives me one more button push of control and understanding when I'm working through the program at the machine for the first time.

    The 2nd tool is a copy and paste of the first. I've altered the color of the items in the second tool that were changed from the first. Hardly much work when you look at it, especially when you consider that you can also use a basic "replace" function to handle the subroutine number changes. Just to be clear, a master program like this can create pretty much any part you can come up with. In multiples.

    T8M6 (3/4 END MILL 2LOC)
    G17G20G40G49G54G80G90G98

    G0X2.125Y-1.22
    G43Z0.1H8S7194M3T9
    M8
    M98P71
    /G55
    /M98P71
    /G56
    /M98P71
    /G57
    /M98P71
    /G58
    /M98P71
    /G59
    /M98P71
    /G54P1
    /M98P71
    /G54P2
    /M98P71
    /G54P3
    /M98P71
    G54P4
    M98P71
    G0Z1.
    M9

    T9M6 (1/2 END MILL)
    G17G20G40G49G54G80G90G98

    G0X-0.26Y-2.5967
    G43Z0.1H9S8252M3T6
    M8
    M98P72
    /G55
    /M98P72
    /G56
    /M98P72
    /G57
    /M98P72
    /G58
    /M98P72
    /G59
    /M98P72
    /G54P1
    /M98P72
    /G54P2
    /M98P72
    /G54P3
    /M98P72
    G54P4
    M98P72
    G0Z1.
    M9

    When someone asks if manual program experience is helpful, I can only answer with a resounding yes. What I've been reading in this thread and others tells me so over and over.

    Dave

  13. Likes DavidScott liked this post
  14. #33
    Join Date
    Aug 2008
    Location
    Philadelphia,PA
    Posts
    125
    Post Thanks / Like
    Likes (Given)
    17
    Likes (Received)
    10

    Default

    For the record I am willing and do the editing to the post so all the noise is eliminated. But I find it hard to not want the ability to get the post to not repeat a program over and over. It is just a waste of time and energy. I figure the more times I can prevent the need for hand coding the more I am likely to avoid a mental error or finger error.

  15. #34
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    272
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    86

    Default

    Quote Originally Posted by EnginCycles View Post
    For the record I am willing and do the editing to the post so all the noise is eliminated. But I find it hard to not want the ability to get the post to not repeat a program over and over. It is just a waste of time and energy. I figure the more times I can prevent the need for hand coding the more I am likely to avoid a mental error or finger error.
    No I hear you EnginCycles. What you go through would drive me nuts as well.

    I suppose for anyone that generally runs post processor based programs, any finger punching could leave a feeling of apprehensive. I guess I'm used to it because of manual programming being the norm. There is a final check I do in all programs. I'll quickly scroll through the whole thing and make sure the tool T number is matched by the following H number and the next tool T number matches the tool that follows. Getting an H number that doesn't match the T before it is my biggest fear, as both are typed in manually, and the wrong tool length offset... well... I'm sure everyone already knows what that will possibly get you.

    Dave

  16. #35
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,749
    Post Thanks / Like
    Likes (Given)
    316
    Likes (Received)
    1828

    Default

    Quote Originally Posted by 13engines View Post
    Not here to get into an argument about the virtues of full on CAM to post processor program generation compared to CAM aided manual programming, but in reading through this post and seeing the fretting and trials and tribulations of those so deeply stuck in and/or reliant on CAM and posts, really makes me glad to have the ability to program manually.
    While all that is correct, I think the OP's question was more along the line of how does one approach multiple part programming.
    Yes, the discussion has taken a turn towards what their CAM can or cannot do, but as far as I understood the OP, his dilemma was more along the line
    that do you draw multiple parts and program it as one, or do you program one and spread it to the multiples you have.

    The answer to that is that it depends on the part.
    In my case:
    1: If I have one piece of material to make multiple pcs, I likely draw and program it as one.
    2: If I have individual slugs of material for each finished piece, I write a single program for one, and then multiply it as needed.

    No matter what though, regardless of Manual or CAM generated program, I always, always, always write the first program for a single instance.
    Then, when all is good and I finally get my Gizmo, I just pour as much water over it as I need to get the desired number of parts per program and I won't feed them after midnight.

    Now, about the ability to manually doing it, you are absolutely correct that it is pretty darn simple to do, let it be a FingerCAM or AnyCAM generated program.
    BUT!
    When there are solutions such as FeatureCAM's Multi Part capability ( as mentioned by Wheelie ), one would almost not ever want to manually
    program anything that may turn out to be a multiple part program.
    And yes, ADSK is working very hard at permanently ruining FeatureCAM, but the odd thing is that Fusion has (apparently) gotten none of it's multipart features.

    Finally about your code...
    If you're dealing with an old Fanuc control, then your approach is the only way to go.
    OTOH if you have an I-series, then ( as far as I am concerned ) your G98 calls should have a Q and not a P word.
    I absolutely HATE having multiple programs for the same fucking part!!!

  17. #36
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    272
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    86

    Default

    Quote Originally Posted by SeymourDumore View Post
    While all that is correct, I think the OP's question was more along the line of how does one approach multiple part programming.
    Yes, the discussion has taken a turn towards what their CAM can or cannot do, but as far as I understood the OP, his dilemma was more along the line
    that do you draw multiple parts and program it as one, or do you program one and spread it to the multiples you have.
    Earlier I had chimed in on the original question, but yes this thread since went south of the OP's thoughts. Yet not surprising seeing that the post originated in the CAD/CAM forum section. I couldn't help myself from responding to all the dismay, which to me lay just outside my scope of comprehension, considering what all that dismay was about and how easily remedied.

    Finally about your code...
    If you're dealing with an old Fanuc control, then your approach is the only way to go.
    OTOH if you have an I-series, then ( as far as I am concerned ) your G98 calls should have a Q and not a P word.
    I absolutely HATE having multiple programs for the same fucking part!!!
    I never knew that about using Q instead of P and what it relates to. My newest control is an 18i on a lathe, which is also new to me, and I haven't yet gotten to writing deeply sub-programmed programs. Though let me suggest that you can still do the Q type thing on older controls, as long as you have the full keypad and can find a comma (,) on it. I sure hate to see you living with all that hate over something so familiar and needed with Fanuc controls for so long as subroutines separate from the main program.

    Take all the subs and line them up one after the other at the end of the main program and copy them all to and from the control as a group that exists together in a single file. (Technically they can be in any order, function or number wise.) I'm not at the shop now so can't verify the exact syntax, but if I'm remembering correctly, just separate the program parts with a line space and add the % or : at the head of each program or sub. (Still using normal program naming convention for each part like O2441 for example.) After the copy, you'll find all your programs sitting individually and correctly named and numbered on your machine control and completely reachable by M98. When you're done with the job and want to copy it back to a hard drive for safe keeping, just use the normal "copy range" function like O2440,O2453 for example. They'll all end up in a single file that can be copied back to the control in the future. (I use dnc4u transfer software, but I don't believe this has anything to do with how this works.) The only thing this idea asks for is that you keep the program parts sort of grouped number wise. How tightly all depends on how many and what numbered programs are usually left on the control. Not that it would technically create problems copying subs or program parts form other part programs, (as the main program would never call them anyway) but I doubt anyone would want to do that on purpose. I'm not sure if there are working limits to this on very old controls. It wouldn't surprise me if a control that had no comma could still accept grouped file input. (Tried it. It does. OMC) At least that would have half the battle won.

    Hope this helps fight off the hate. :-)
    Dave

    Edit: Looks like the file starts and ends with the % sign like any other. So there will be two at the beginning.
    File I checked look like this. (As returned from control.) As most know % = : in Fanuc

    %
    :O2440 (FIRST PROGRAM HERE)
    - - - -
    M30
    :O2442 (REST OF PROGRAMS)
    - - - -
    M99
    :O2453 (LAST PROGRAM HERE)
    - - - -
    M99
    %
    Last edited by 13engines; 11-28-2019 at 03:45 PM. Reason: Update on correct syntax

  18. #37
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,749
    Post Thanks / Like
    Likes (Given)
    316
    Likes (Received)
    1828

    Default

    Quote Originally Posted by 13engines View Post

    I never knew that about using Q instead of P and what it relates to. My newest control is an 18i on a lathe, which is also new to me, and I haven't yet gotten to writing deeply sub-programmed programs. Though let me suggest that you can still do the Q type thing on older controls, as long as you have the full keypad and can find a comma (,) on it. I sure hate to see you living with all that hate over something so familiar and needed with Fanuc controls for so long as subroutines separate from the main program.
    With G98 P1234 call, there must be a registered, separate program in the control.
    With a G98 Q1234, there must be a block# N1234 in the SAME program.

    IOW, a G98 P call is a subPROGRAM call, whereby a G98 Q is a subROUTINE call.

    And as far as I know, Fanuc made the subroutine call (Q) possible starting with the I series controls and was not an option on the older ones.

  19. #38
    Join Date
    Aug 2008
    Location
    Philadelphia,PA
    Posts
    125
    Post Thanks / Like
    Likes (Given)
    17
    Likes (Received)
    10

    Default

    So all this P and Q got me searching for options within the post drop down menu. I tried for the heck of it subroutine patterns which I never did and had no idea what it is. Well it is how all my problems are solved! If you pick subroutine PATTERNS it does a subroutine and only writes the program once. Why in the world do you need to select patterns? This makes little sense to me but neither does "smoothing" which sounds to me like it would make the code longer but it is hardly that. This thread saved me so many hours of hand coding for the future.

    THANKS!

    -Drew


Tags for this Thread

Bookmarks

Posting Permissions

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