Thread: Bridgeport Manual to CNC conversion...

Page 30 of 30 FirstFirst ... 20282930
  1. #291
    Yep, i made a point of not changing anything else at all, just double the acceleration figure in motor tuning, verified my following errors in pid tuning then run the code. Following error did not alter which is good.

  2. #292
    Quote Originally Posted by AndyGuid View Post
    Just to clarify please, that the only difference between the Before and After results above was an increase in acceleration in motor tuning?

    That's quite amazing!
    Andy Acceleration can make huge difference to how machine performs, not only in quality of cut but also Cycle times.

    Often on Smaller jobs with lots of very short moves ie: V carving engraving setting Accelleration higher and lowering velocity can increase cycle times quite drasticly.
    In daves case the cause was being set to constant velocity mode G64. Meaning the control trys to maintain constant feed rate around corners. Obviously the laws of physics come into play at some point and becomes impossible to maintain this rate around tight corners.
    Simplisticly put It does this by overlapping Accelleration needed for the new move with De-accelaration of the current move and the point they meet is when corner rounding occurs.
    So obviously if acceleration is low then de-acceleration must happen sooner and the point they meet is further up the road. Think of it like car with poor skinny tyres and throttle stuck on.!! You turn sooner to get around corner else you crash.!! . . Having higher acceleration is like Car with brand new wide tyres so can turn later.

    If you want to follow the Tool path exactly you'd use G61 Exact stop mode. Which goes exactly from point A to B and repeats for each following move. The down side of this can be very jurky movement and pause at each start/end point. If Cam software creates Arcs with tiny little lines G61 with high feedrate can shake machine to pieces.!
    To see this in action Try some G-code which doesn't have G64 at the top or change to G61. If doesn't have in code Type G61 in MDI before running.
    Last edited by JAZZCNC; 30-11-2016 at 08:55 PM.

  3. The Following User Says Thank You to JAZZCNC For This Useful Post:


  4. #293
    Hi all,

    been a while since this thread

    For those who don't know, my Bridgeport was rebuilt with servos and larger motor, plus i added an auxiliary high speed spindle for aluminium work. The job in hand is shown in the pictures below, 5mm Aluminium, lots of holes and intricate features. I use 2mm single-flute and 5mm single-flute carbide tools for these.

    Previously, I had already built a custom mini-mill to make these (and learn CNC) and still have this (its currently up for sale but no takers yet).

    My reason for adding the aux spindle to the Bridgeport was two-fold - one, to save space and two, to make more use of the very expensive Bridgeport conversion which would otherwise only see intermittent use.

    Now, when doing these on the Bridgeport, I am seeing bad vibration or chatter on the tool, it appears to be vertical oscillation but tonight also suffered bad enough radial oscillation to break a 5mm tool ! When it goes into oscillation it makes you jump as its very noisy and you instantly know it will end badly either in poor finish or broken tooling. Tonight I was testing tool sent from my supplier as a "Better" option this was a two-flute carbide, probably the reason for the breakage as two-flute tools need a more rigid setup.

    So, something is not happy - my reservation is the spindle mount (shown below) - its canted out over to one side and although it's clamped to the quill and into an R8 collet in the main spindle, it must be allowing deflection from the cutting forces.

    Ok, so I have a bad situation, is there a way forward here?

    Obviously I can take the dust-sheets off the mini-mill and carry on but I just don't have the space long-term and wanted to make more use of the Bridgeport as mentioned. I really want a one-size fits all solution here.

    If I run the small tooling on the BP main spindle at 3000rpm (top whack) the run time per part-set will go from about 30minutes to several hours probably - feed rates go from 900mm/min to 25mm/min so i don't think thats an option - it needs more RPM's.

    What can be done here guys???

    Spindle-speeders?? I have seen these but they have mixed reviews and i doubt they would like a 5mm tool much as mostly used for engraving etc.

    One idea I quite like is to spin the ram on the BP around and build a custom Z-axis completely, and mount it where the BP slotting head normally sits. This could be built as heavily as desired with linear guides and a servo or stepper etc.

    Click image for larger version. 

Name:	dIMG_1682.JPG 
Views:	190 
Size:	793.8 KB 
ID:	20574

    Click image for larger version. 

Name:	dIMG_1681.JPG 
Views:	53 
Size:	1.42 MB 
ID:	20575

    Click image for larger version. 

Name:	dIMG_1680.JPG 
Views:	45 
Size:	1.16 MB 
ID:	20576

  5. #294
    m_c's Avatar
    Lives in East Lothian, United Kingdom. Last Activity: 12 Hours Ago Has been a member for 8-9 years. Has a total post count of 1,703. Received thanks 176 times, giving thanks to others 5 times.
    The first thing that springs to mind, is how much play is in the quill?

    By bolting onto the quill the way you have, any play in the quill will be greatly magnified at the second spindle, so it's probably not taken much extra wear to go from tolerable to a problem.

    Creating a new Z-axis assembly sounds like the best long term solution.
    Avoiding the rubbish customer service from AluminiumWarehouse since July '13.

  6. #295
    Yes, I was working through this on the drive to work this morning ;)

    There will be play, must be or it would seize, plus being umpty years old i guess there will be a measurable amount.

    The setup is perfect on the 2mm tools or engraving etc so it seems somewhere between 2mm and 5mm tooling is a point where cutter force and reaction come into play and bite me in the arse.

    I am leaning towards a fully custom Z axis now, this brings about its own set of issues of course -

    Will have to move machine away from rear wall,
    ..Can't move machine away from rear wall as the head hits the roof truss,
    ....Will have to radically modify roof truss to make clearance,
    The list goes on - sometimes i hate my garage shop.

    Next is - steel or aluminium build??

    I am visioning it as being just a larger version of the Z axis on my mini-mill so two flat plates with rails and a screw sandwiched between, servo motor to drive and a toothed belt?

    It does not need massive rails as the biggest tool is likely to be 5-6mm max so probably the same 20mm HiWin and a 1605 screw, maybe use stuff with a pre-load this time??

    The hard part is working out the connection to the rear of the ram and where to put strengthening trusses/plates etc - the rear of a BP ram is a spigot maybe 50mm tall, 110mm wide and 100mm deep with a 20mm hole central - that is all i have to mount off of.

    So, something like 25mm tooling plate all round or go steel and weld etc where possible.??
    Last edited by Davek0974; 03-02-2017 at 11:02 AM.

  7. #296
    m_c's Avatar
    Lives in East Lothian, United Kingdom. Last Activity: 12 Hours Ago Has been a member for 8-9 years. Has a total post count of 1,703. Received thanks 176 times, giving thanks to others 5 times.
    My thought would be to weld the BP side, as it gives you more flexibility in terms of bracing/reinforcing. You would ideally need to stress relief it before doing the final machining for the rails, to minimise any long term stability issues.
    Avoiding the rubbish customer service from AluminiumWarehouse since July '13.

  8. #297
    So, welded interconnect plate, relieve, then machine square etc.

    Then build the motion parts in Alu ?

  9. #298
    Hmmm,

    Just been playing speeds & feeds for my single flute 5mm tool...

    Manufacturer specs...
    12k Rpm
    2.5m DOC
    1800mm/min feed - insane i think?

    My previous settings...
    12k rpm
    2.5mm DOC
    900-1000mm/min feed

    F&S Calculator recomendations...
    12k rpm
    1.8mm DOC
    280mm/min feed - much lower ?

    Maybe these lighter settings will be better?

    Its only the bigger tool that has issues so does seem to be a stress problem, I will also attach a bungee cord to the head to try and remove any rotational slack in the quill.

  10. #299
    Ok, did some tests, first was to measure slack in the z axis at the adaptor in line with the high speed spindle - I have 0.02mm vertical (with reasonable force) and 0.15mm rotational around the quill - no doubt the source of my trouble.

    Left cuts in the first picture below was at the feed recommended by my S&F calculator shown in the last post, 2 passes of 1.25mm ea, top cut is with me applying pressure to the motor while cutting to remove slack, the lower cut is with it running free as normal.

    Both cuts look fine, no burr on the lip and pretty much perfect.

    The right cuts in the first pic show results of a single 2.5mm DOC pass, same feed rate, again with hand pressure on the top pass and free on the lower.

    Both cuts are acceptable this time but they show signs of vibration on the bottom surface - this is not an issue here as this tool is a roughing tool and will cut right through on these parts.

    the second pic is just a closer view of the vibration on the second cuts.

    Seems I just have to back off on the fast pedal a bit and let her do her thing, plus fit a bungee cord to remove the slop.

    Click image for larger version. 

Name:	dIMG_1684.JPG 
Views:	190 
Size:	477.4 KB 
ID:	20590

    Click image for larger version. 

Name:	dIMG_1685.JPG 
Views:	187 
Size:	489.2 KB 
ID:	20589

  11. #300
    Quote Originally Posted by Davek0974 View Post
    Ok, did some tests, first was to measure slack in the z axis at the adaptor in line with the high speed spindle - I have 0.02mm vertical (with reasonable force) and 0.15mm rotational around the quill - no doubt the source of my trouble.

    Left cuts in the first picture below was at the feed recommended by my S&F calculator shown in the last post, 2 passes of 1.25mm ea, top cut is with me applying pressure to the motor while cutting to remove slack, the lower cut is with it running free as normal.

    Both cuts look fine, no burr on the lip and pretty much perfect.

    The right cuts in the first pic show results of a single 2.5mm DOC pass, same feed rate, again with hand pressure on the top pass and free on the lower.

    Both cuts are acceptable this time but they show signs of vibration on the bottom surface - this is not an issue here as this tool is a roughing tool and will cut right through on these parts.

    the second pic is just a closer view of the vibration on the second cuts.

    Seems I just have to back off on the fast pedal a bit and let her do her thing, plus fit a bungee cord to remove the slop.

    Click image for larger version. 

Name:	dIMG_1684.JPG 
Views:	190 
Size:	477.4 KB 
ID:	20590

    Click image for larger version. 

Name:	dIMG_1685.JPG 
Views:	187 
Size:	489.2 KB 
ID:	20589

Page 30 of 30 FirstFirst ... 20282930

Similar Threads

  1. Milling machine CNC conversion - keep hand wheels for manual operation?
    By birchy in forum Milling Machines, Builds & Conversions
    Replies: 5
    Last Post: 23-10-2016, 08:29 PM
  2. Manual autochanger problems.
    By Saracen in forum Lathes, Lathe Rebuilding & Conversions
    Replies: 1
    Last Post: 05-02-2015, 12:14 AM
  3. WANTED: Centec 2A manual
    By Web Goblin in forum Items Wanted
    Replies: 0
    Last Post: 03-09-2012, 09:56 AM
  4. Translating the manual
    By Robin Hewitt in forum Moulding Machines
    Replies: 22
    Last Post: 01-09-2012, 01:21 PM
  5. Bridgeport Conversion
    By Tony Goodwin in forum Bridgeport Milling Machines
    Replies: 0
    Last Post: 08-08-2011, 08:11 AM

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
  •