567,250 active members*
4,451 visitors online*
Register for free
Login
Page 1 of 5 123
Results 1 to 20 of 85
  1. #1
    Registered
    Join Date
    Dec 2005
    Posts
    495

    Fusion 360 post for Bridgeport DX-32.

    Has anyone re-worked the generic Bridgeport post for Fusion 360 to work with the DX-32 control? The generic post isn't posting correctly. Figured I'd ask before I re-worked it.

  2. #2
    Registered
    Join Date
    Dec 2005
    Posts
    495

    Re: Fusion 360 post for Bridgeport DX-32.

    I found this thread by samtransam: https://forums.autodesk.com/t5/hsm-p...ght/true#M2308

    The thread is fairly old. The post has some details I haven't seen. The changes he made appear in the latest generic bridgeport post. Samtransam states an arrow symbol (writeln("\u0011") is required at the start of the file but I've never seen that symbol in my posts from VisualMill. Also, his comments are in single quotes followed by a semi-colon. I believe this is legal on the DX-32 but the programming guide only lists comments as starting with a semi-colon. I've always done my comments starting with a semi-colon. He also ends the program, following the M2 block, with a block containing the letter E, for end I presume. It also contains an :O filename like :O1001 which in Fanuc style, I've never used this on my TC-3.

    For my post I started with the current generic bridgeport post. Removed the arrow symbol at the top and E block at the bottom. I switched tapping to rigid using M29. I added a switch to the properties so the default rigid tapping can be turned off for floating tap. Left handed tapping was disabled in the post code so I reworked it to allow left handed taps. This is not tested but I assume the G84 direction is dependent on the spindle direction M3/M4 instead of calling left handed as G74 like some controls. Left handed tapping is evaluated based on the tap being left handed in the tool library. I used Fanuc style comments as they are easy to read... and I recycled my code from my Fanuc post. I also removed the semi-colon at the end of each block. I changed the post to allow non-numeric names. And removed the :0 file name like :01001.

    I added a section that I use in all my posts to include the date , fusion version, filename, and username of who posted the file. I work in a multi-user environment and this helps at the machine. Date is UTC.
    ;(Sunday, July 09, 2017 1:43:33 AM)
    ;(Fusion 360 CAM 2.0.3174)
    ;(msr_cap v3)
    ;(forhire)

    UPDATE: I did a dry run of three separate operations. One right hand rigid tapping, left hand rigid tapping, and thread milling (helical). All three appear to have run flawlessly! The only change I required is that my TC-3 would only see *.TXT files in the file manager so I had to change the extension from *.NC to *.TXT. I should have known because I've always posted filename.txt. Easy fix. I deleted the original attachment and uploaded a new one.

  3. #3
    Registered
    Join Date
    Dec 2005
    Posts
    495

    Re: Fusion 360 post for Bridgeport DX-32.

    Realized WCS was disabled in the generic bridgeport post I started with, as a result, no G54 to G59 would be honored despite entering a value in CAM setup.

    Here is the updated post.
    Attached Files Attached Files

  4. #4
    Registered
    Join Date
    Dec 2005
    Posts
    495

    Re: Fusion 360 post for Bridgeport DX-32.

    nlh made a number of suggestions via PM based on his Bobcad post. I have integrated those changes into the current post.

    1) When using serial DNC a percent symbol is required at the top and bottom of the code. Added the % symbol. This is the same as Fanuc and others. Interestingly, I DNC from the hard drive and the symbol isn't required.

    2) Set the init preamble to match the manual.
    "The active preparatory function (G code) commands are reset back to initialized conditions.
    The following G codes are set: G0, G17, G30, G40, G45, G54, G70 or G71, G72, G75, G90, G96"

    In addition I included G80 for good measure. Fusion 360 already defaulted to G44 instead of G45 which is constant surface feed when using cutter comp. Open to suggestions on this one.

    This it the updated init:
    N10 G0 G17 G30 G40 G44 G72 G75 G80 G90 G96
    N11 G70

    3) Added M9, M5, G90 and a % symbol at the end in addition to M22.

    Output looks like this:
    N128 M9
    N129 M5
    N130 G90
    N131 M22
    %

  5. #5
    Gold Member
    Join Date
    Sep 2009
    Posts
    1856

    Re: Fusion 360 post for Bridgeport DX-32.

    If you wont to change the G44 to G45 just change it or put a if statment in with a selection so you can change it in the pre post dialog
    http://danielscnc.webs.com/

    being disabled is not a hindrance it gives you attitude
    [SIGPIC][/SIGPIC]

  6. #6
    Registered
    Join Date
    Dec 2005
    Posts
    495

    Re: Fusion 360 post for Bridgeport DX-32.

    Quote Originally Posted by daniellyall View Post
    If you wont to change the G44 to G45 just change it or put a if statment in with a selection so you can change it in the pre post dialog
    G44 is the default in the generic bridgeport post. I have no issue either way. Obviously someone thought it was preferred. I just noticed the default in the manual is G45. My visualmill post doesn't include G44/g45 and I don't think it was included in nates's bobcad post either. Being that it is hard coded in the fusion360 post at present, it likely needs to be toggled when using cutter comp. In reality because it only affects cutter comp maybe changing it to default makes the most sense. Please let me know what you'd like.

    Here is the manual snippit. It looks like it could be useful.
    Click image for larger version. 

Name:	g44g45.PNG 
Views:	1 
Size:	84.4 KB 
ID:	367724

  7. #7
    Member
    Join Date
    Oct 2005
    Posts
    420

    Re: Fusion 360 post for Bridgeport DX-32.

    I for got to add in my PM that I would normally put a G45 at the top if anything. I believe this code only comes into play when using cutter comp. On the other hand, I have not noticed a big difference either way (G45 vs G44). I typically only use cutter comp to dial in part dimensions. So probably would not see big feedrate changes on such small offsets (i.e., .001" - .02"). I will offset for cutter radius within the CAM software.

    If you could give me some quick instructions, I think I could probably edit the post for G45 vs G44 on my end. Might be quicker/easier than uploading a completely new post just for that edit.

    Great stuff forhire!

    I need to add java script to my list of things to learn, or at least develop a working knowledge of.

  8. #8
    Member
    Join Date
    Oct 2005
    Posts
    420

    Re: Fusion 360 post for Bridgeport DX-32.

    For those that are following this thread, I wanted to post the text of my PM to forhire. It is just a cut and paste.

    "That post looks like it should work fine on my end. The only major differences I see is that I typically have a few more G-Codes at the starting block. Typically it will read "G0 G40 G90 G80 G17 G96". I've done that for years on all my machines, more out of habit but also for safety. Just makes sure the control is clear and ready to run the program.

    The G96 is DX32 specific. It cancels a G97 (also DX32 specific) which is a work coordinate shift. I find I use a G97 alot. In certain situations I run a G97 and then a Z figure that will put my tools a safe distance above my part just to test run. Other times will use a G97 to fine tune my part dimensions.

    Here is a snippet of sample code that I output from Bobcad. I would post the whole thing but can't figure out attachments within PM's.

    :100
    ;2-AXIS SAMPLE.NC
    ;TUE. 07/11/2017 07:25PM
    ; BRIDGEPORT DX-32 VMC
    T1 /3. /.5
    G70
    G0 G90 G80 G17 G40 G96
    ;Machine Setup - 1 Pocket
    ;FEATURE 2 AXIS
    T1 M6
    S595 M3
    G54
    X2.0269 Y2.1861 Z1.
    M8
    G0 Z.2
    Z.1
    G17 G13 X1.9837 Y2.1938 Z.0931 R.125 F3.34
    X1.8587 Y2.0688 Z.0863 R.125

    and the ending blocks:

    G0 Z.1
    Z.2
    Z1.
    M5
    M9
    G90
    M22

    That is completely unedited. I modified a stock bobcad DX32 post to within probably 80-90%. At this point I need to do something with that T callout, but have not been able to get it to output a semicolon in front. So I add in by hand after. I will also add a bunch of notes at the top of the program....setup notes, tool notes, material, jigs/fixtures, etc.

    If I use a G97, I will manually add that after the work offset.

    I hate all the consecutive Z moves (Z1., Z.2, Z.1, etc) and will streamline those as best as possible. However, not much I can do about that in the bobcad post, as it seems to be built within the feature, not the post processor.

    I will also remove that ":100". I will put a "%" at the very top and bottom. The one at top may not be needed, but I add it out of habit. I can't send the program to the machine correctly via RS232 unless I have the one at the end of the program.

    Another thing to note, semi-colons are typically what the DX32 uses for comments. You can also use a ' at the beginning of a comment which the control will output to the screen after it reads it. It can be used to aid an operator. It's a little clunky but works.

    I'm pretty much a "one man band" shop, so I can get away with the manual edits. A bigger shop would probably need a better post that they didn't have to micromanage as much.

    Very interested in trying out your Fusion post! I can see how beneficial Fusion will be for certain jobs over bobcad.

    Nate

  9. #9
    Registered
    Join Date
    Jun 2003
    Posts
    202

    Re: Fusion 360 post for Bridgeport DX-32.

    This post is a good example of why post processors are OLD SCHOOL ... new out-of-the-box thinking :
    Why CAD/CAM Post Processors Are Old School And Obsolete | The Kipware Blog

  10. #10
    Registered
    Join Date
    Dec 2005
    Posts
    495

    Re: Fusion 360 post for Bridgeport DX-32.

    Quote Originally Posted by BlueChip View Post
    This post is a good example of why post processors are OLD SCHOOL ... new out-of-the-box thinking :
    Why CAD/CAM Post Processors Are Old School And Obsolete | The Kipware Blog
    Advertisement? Hardly anything new, NCPlot (and others) will do these kind of "cleanup" conversions, and it's a great back plotter also. Yes I watched the video. I have a number of similar tools, including scaling tools. I my opinion messing with g-code is way more cumbersome and risky than re-posting clean from cam. If you have proven posts then re-posting to different machines is a non issue. One issue I see with g-code manipulation is that they rarely take into account tool library variations between machines. At present I maintain 8 post processor for my environment, all started with generic posts but none were 100% to my liking. This DX32 post was by far the most work because rigid tapping, LH tapping, and WCS were all missing from the generic post. Now that it's clean... I can post with confidence.

  11. #11
    Registered
    Join Date
    Dec 2005
    Posts
    495

    Re: Fusion 360 post for Bridgeport DX-32.

    Quote Originally Posted by nlh View Post
    If you could give me some quick instructions, I think I could probably edit the post for G45 vs G44 on my end. Might be quicker/easier than uploading a completely new post just for that edit.
    Click Open Config on the post dialog and it will open the post in the default editor. Scroll down to line 251 and change gFeedModeModal.format(44) to gFeedModeModal.format(45) (bolded)
    251: writeBlock(gFormat.format(0), gFormat.format(17), gFormat.format(30), gFormat.format(40), gFeedModeModal.format(45), gFormat.format(72), gFormat.format(75), gFormat.format(80), gAbsIncModal.format(90), gFormat.format(96));

    I attached my latest post with the value changed. Enjoy!
    Attached Files Attached Files

  12. #12
    Member
    Join Date
    Oct 2005
    Posts
    420

    Re: Fusion 360 post for Bridgeport DX-32.

    Thanks forhire!

  13. #13
    Member
    Join Date
    Oct 2005
    Posts
    420

    Re: Fusion 360 post for Bridgeport DX-32.

    Here is another one forhire.

    I typically only use sequence numbers at the beginning of each feature that calls out a tool change. For instance, if I'm calling up tool 3, I will have an "N3" at the beginning of the sequence for T3.

    Helps when I need to restart the program at a given tool. Technically I don't need to do this with the DX32 as it allows restarting based on searching for seq numbers (N) or by tool (T) (There is also a third item to search by I think, but don't recall of top of my head). However, I'm used to restarting by "N" from the other controls I've run over the years.

    Bobcad has a feature in it's posting that allows me to do this. I don't see anything obvious in the Fusion 360 post that would allow this. Any idea's?

  14. #14
    Registered
    Join Date
    Dec 2005
    Posts
    495

    Re: Fusion 360 post for Bridgeport DX-32.

    Quote Originally Posted by nlh View Post
    Bobcad has a feature in it's posting that allows me to do this. I don't see anything obvious in the Fusion 360 post that would allow this. Any idea's?
    Good point. My MAPPS on the Mori lathe numbers the operations this way. Darn handy. It shouldn't take much, I'll look at it tonight.

  15. #15
    Registered
    Join Date
    Dec 2005
    Posts
    495

    Re: Fusion 360 post for Bridgeport DX-32.

    Quote Originally Posted by nlh View Post
    I typically only use sequence numbers at the beginning of each feature that calls out a tool change. For instance, if I'm calling up tool 3, I will have an "N3" at the beginning of the sequence for T3.
    I put a switch to count the operations called numberOperations. It uses the sequenceNumerber variables, like start number and increment. Right now it does all the functions in order. I don't know if matching the tool number to the operation makes sense as sometimes T3 might be used in the 1st, 3rd, and 10th operation.

    Be aware that if showSequenceNumbers=true then it will over ride numberOperations. All operations must have a name/comment for this to work. I didn't skip the operations with a tool already selected. I put the operationNumber on the same line as the operation comment, it was logical and similar to my mori post.

    Post up some code and see if this is workable. This is from the first operation.

    G70
    N1 ;(2D Pocket)
    M9
    T4 M6

  16. #16
    Registered
    Join Date
    Dec 2005
    Posts
    495

    Re: Fusion 360 post for Bridgeport DX-32.

    Nate, here's an interesting one. Today I was running my first production part and kept getting an error #10 Internal Addressing Error when attempting to enter run mode after loading my program. Same program I tested with last week. Turns out if I have the percent symbol (%) at the top and bottom of the program it generates the error. Removed the symbol and all was well. Any ideas? I know it is required for serial dnc. If you load a program from floppy with the percent symbol do you get the error? I guess I hadn't tested after the addition.

  17. #17
    Member
    Join Date
    Oct 2005
    Posts
    420

    Re: Fusion 360 post for Bridgeport DX-32.

    Now that you mention it, when I send a program from my laptop to the dx32 (via RS232), those symbols seem to get automatically removed once the control receives the program. Seems for me, it is needed by my DNC program to properly send and receive. I believe the Internal Addressing Error is due to the control not recognizing the % as processible code. I bet if you put those symbols back in and then put a semi-colon in front of each, the control would not alarm. I've had similar error's when forgetting to have a semi-colon to start a comment line.

    I haven't had time to try any code on my machine yet, but from the sample code I've posted so far, it looks good.

    Only thing I haven't checked, and just thought about yesterday, was cutter comp and how it posts in a program. If I get a chance I'll check that tomorrow.

    I've been spending time going thru tutorials and watching YouTube vids. Trying to learn enough to get comfortable with Fusion. So far I really like it!

  18. #18
    Registered
    Join Date
    Dec 2005
    Posts
    495

    Re: Fusion 360 post for Bridgeport DX-32.

    Quote Originally Posted by nlh View Post
    Now that you mention it, when I send a program from my laptop to the dx32 (via RS232), those symbols seem to get automatically removed once the control receives the program. Seems for me, it is needed by my DNC program to properly send and receive. I believe the Internal Addressing Error is due to the control not recognizing the % as processible code. I bet if you put those symbols back in and then put a semi-colon in front of each, the control would not alarm. I've had similar error's when forgetting to have a semi-colon to start a comment line.
    I was actually surprised it complained.I added a parameter called serialDNC that is normally false to my post. Of course it can be changed to true in the post if that's your default. I don't know if treating it like a comment would work. I believe is that it has to be the top most symbol on it's own line. Treating it as a comment is an easy solution, if it works. Can you test that?

  19. #19
    Registered
    Join Date
    Dec 2005
    Posts
    495

    Re: Fusion 360 post for Bridgeport DX-32.

    I tried a lot of variations to keep the percent symbol in place without generating an error in the control. You may want to see if your DNC software can send the file control characters for you. In any case I added a serialDNC file control option. See this latest post. I ran some alternate WCS while drilling and rigid tapping today. So far the post is working well.

    Change line 52 it you prefer the symbol by default.
    52: serialDNC: false // include percent symbol top and bottom
    Attached Files Attached Files

  20. #20
    Member
    Join Date
    Oct 2005
    Posts
    420

    Re: Fusion 360 post for Bridgeport DX-32.

    Sorry I wasn't able to get back to you yesterday. I was able to test a couple different things with that "%" symbol. First I manually added them to the program already loaded into the machine. 1 at top and 1 at bottom. Upon saving and returning to the run screen immediately got an error. Parser #4 Internal Addressing Error. I then added a semi-colon in front of the top % and it worked fine. The bottom one seemed to have no effect either way.

    I'll check out my DNC software and see if there are some settings that can be changed. I've just gotten used to all my other machines needing it, guess I've never given it any thought.

    I get used to doing things a certain way, and if I'm having positive results, take it for granted.

Page 1 of 5 123

Similar Threads

  1. Dynatorch post for Fusion 360?
    By forhire in forum DynaTorch
    Replies: 4
    Last Post: 05-24-2022, 03:46 AM
  2. Replies: 0
    Last Post: 08-23-2016, 08:01 PM
  3. fusion 360 post?
    By mikethemachine in forum Post Processor Files
    Replies: 1
    Last Post: 05-23-2016, 06:01 PM
  4. Tormach Post and Fusion 360
    By grimms3 in forum Tormach Personal CNC Mill
    Replies: 8
    Last Post: 10-20-2015, 04:58 AM
  5. Fusion 360 Post
    By wildwhl in forum Tormach Personal CNC Mill
    Replies: 10
    Last Post: 08-27-2015, 05:10 AM

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
  •