Need Help! Spoil Board


Results 1 to 16 of 16

Thread: Spoil Board

  1. #1
    Registered
    Join Date
    Jun 2017
    Location
    United States
    Posts
    54
    Downloads
    0
    Uploads
    0

    Default Spoil Board

    I am purchasing a new CNC machine with a 6m Syntec controller. It has 3 spindles instead of a tool changer. I am only buying this model because its the only machine available at the moment.This is the first time I will be using Syntec. This machine DOES NOT come with tool touch off sensor but I would still like to zero off the actual vacuum table itself and then add the spoil board thickness to it so that the top of my spoil board is my Z0. (I know I have to set my toolpath in VCarve Pro 8.5 to zero at the bottom of material). I would like to be able to fly cut my spoil board and add the new value as I go along so I do not have to zero my 3 spindles every time I flycut. Any advice would be great. Thanks


    Questions
    1: How do I set the zero as described above?
    2: Does Syntec save my zero so I dont have to do this every time I start up my machine?
    3: Do I even need to mess with parameter 3411 to do this? or is that only for setting the difference between the tool touch off sensor and the actual table.(Remember I do not have a tool touch off sensor)

    Similar Threads:


  2. #2
    Member
    Join Date
    Aug 2009
    Location
    Canada
    Posts
    655
    Downloads
    0
    Uploads
    0

    Default Re: Spoil Board

    Pretty easy, touch off your vacuum table with any tool (pick on that is easy to get a good height with or your flycutter). Enter that absolute value as your tool offset for that tool. Then in the offset screen, make your z offset equal to the thickness of your spoil board. You may need to start at the nominal thickness of the spoil board and move down (by reducing the z offset) until it's flat. After that, you can touch the remaining tools off the spoil board (but then you need to minus the z offset from the absolute value).

    To resurface the spoil board, reduce the offset amount only by say .5mm or 1mm or whatever and do a fly cutter of the table at 0 depth (in Vcarve).

    For example, my grid top table is say -369.02mm for my. 25" cutter.

    My spoil board is currently 8mm (started at about 16mm). If I touch off the top of the spoil board right now, I should get -361.02 then I minus 8 for the spoil board and enter - 369.02 in the tool offset. When first had a new spoil board it would have been top of spoil board -16 (or whatever based on the original thickness).

    Don't worry if you absolute value is way different than mine (I might have screwed it up when I first got it), these are all about the relative spacing.

    Hope that is clear as mud (at least when you have it in house).

    I had a touch off but it was not level and had some give on the mounting so I do it manually anyhow.

    Sent from my LG-D852 using Tapatalk

    In case anyone is wondering, I'm the twin of the other gfacer on cnczone...


  3. #3
    Member
    Join Date
    Aug 2009
    Location
    Canada
    Posts
    655
    Downloads
    0
    Uploads
    0

    Default Re: Spoil Board

    Oh sorry. I only answered 1.

    2) yrs syntec saves it all
    3) not you shouldn't need 3411, which is sort of the same from vacuum table to touch off value (but as you don't plane down your touch off sensor, should never change).

    Sent from my LG-D852 using Tapatalk

    In case anyone is wondering, I'm the twin of the other gfacer on cnczone...


  4. #4
    Registered
    Join Date
    Jun 2017
    Location
    United States
    Posts
    54
    Downloads
    0
    Uploads
    0

    Default Re: Spoil Board

    Do I need to mess around with parameter 3411?



  5. #5
    Registered
    Join Date
    Jun 2017
    Location
    United States
    Posts
    54
    Downloads
    0
    Uploads
    0

    Default Re: Spoil Board

    Where do I enter absolute value as my tool offset?



  6. #6
    Member
    Join Date
    Aug 2009
    Location
    Canada
    Posts
    655
    Downloads
    0
    Uploads
    0

    Default Re: Spoil Board

    Menu - offset setting - tool set.

    Z offset is z external shift

    Sent from my LG-D852 using Tapatalk

    In case anyone is wondering, I'm the twin of the other gfacer on cnczone...


  7. #7
    Registered
    Join Date
    Jun 2017
    Location
    United States
    Posts
    54
    Downloads
    0
    Uploads
    0

    Default Re: Spoil Board

    Why do I only have to touch the first tool to the vacuum table and the other two tools to the spoil board? shouldn't I have to touch off all tools to the vacuum table?



  8. #8
    Member
    Join Date
    Aug 2009
    Location
    Canada
    Posts
    655
    Downloads
    0
    Uploads
    0

    Default Re: Spoil Board

    What you essentially are doing is using a tool as a reference tool then setting things off of it. But just to set up the spoilboard. After that, everything basically references to the spoilboard - which due to the use of the external z shift - is now a variable height.

    You can redo it off the grid whenever you change spoilboards if you like but in practice you likely don't really need to as you likely aren't ever going to get so thin on the spoilboard that it matters.

    You could do all of the tools off the grid if you want but unless you plan to use that exact tooling for the entire time you have the spoilboard on then it doesn't matter. You really just need a value to start with - which is the one tool (the more I think about it, its probably a little easier if that tool is your flycutter but doesn't need to be - I didn't), and then you add the thickness of the spoilboard to the external z shift input. After that, you basically are going off the spoilboard.

    Another example - My tool #1 is -369.02 still. I add the spoilboard which is a nominal 18mm, so I add 17 to the external z shift (as I assume I will need to remove 1mm to get it flat). I then run a program to cut the face of the spoilboard at 0 height (ok not really, I use a material thickness 0.01 and a cut depth of .01").

    At the end of the program I can see it is still not flat. So I change the external z shift to 16.5mm and recut. Now it is flat. My tool 1 when touched off the spoilboard is now (ideally - spoilboards and our ability to set zero vary slightly) -352.52mm.

    Now I want to set tool #2. I lower it to hit the spoilboard (I use a piece of paper and MPG the tool down until it just cuts it). I look at the machine value of (for example) -340.16. I know that tool #1 cut the spoilboard at exactly 16.5mm above its offset value (ie the value of the z shift). So I need to do the reverse and take the -340.16 that I read at the top of the spoilboard and MINUS the z shift. So for tool #2 I would enter an offset of -356.66.

    Same for tool #1 or any other tool as new tooling is put in.

    Part #2: OK now I need to reface the spoilboard. I enter a new z shift amount that is again .5mm-1mm lower (16mm in the above case) and rerun the facing program. As we only changed the external shift, every tool should be still at 0 (in vcarve) when at the top of the spoilboard because none of the underlying values in the tool offset changed. However if you now set up a new tool, you only minus 16mm not 16.5mm from the position you read at the top of the spoilboard.

    Now that is the ideal as I said. Every time you set it off the spoilboard, or even just check it, it will vary a tiny bit. So you have an issue with a tool not cutting at exactly the right depth, just reset it as if it was a new tool.

    Hope that is a little more clear?

    In case anyone is wondering, I'm the twin of the other gfacer on cnczone...


  9. #9
    Registered
    Join Date
    Jun 2017
    Location
    United States
    Posts
    54
    Downloads
    0
    Uploads
    0

    Default Re: Spoil Board

    Thank you for this information, I will reference it when I have the machine in front of me. Is this the place I should ask questions about other Syntec issues. The Company I am buying the machine from no longer supports Syntec so they cannot really help me with it. They will help with the machine but not the controller. During my online research I was unable to find tech support for it. Is Syntec a USA program? Also the machine comes with a movable touch plate but the current owner has never used it. How would I go about configuring this? Is this were Parameter 3411 comes into play. I think I will just do my tool touch off manually but I would like the option?

    Thanks



  10. #10
    Member
    Join Date
    Aug 2009
    Location
    Canada
    Posts
    655
    Downloads
    0
    Uploads
    0

    Default Re: Spoil Board

    Who the heck are you buying it from? Not that I would expect them to be any good at supporting it but they should at least try and support it.

    You can find some information here. I have had some contact with Syntec directly. Syntec is a Taiwanese system and they don't seem particularly geared to the export or non Asian market. The controller itself has been good. Not 100% rock solid as I have crashed it a few times (in the same way usually) but generally really good. Only issues during a program is when it was a DNC program on the network - it started losing it mid program and since then I've moved to downloading them to the syntec directly (I call my temp programs all the same to save space and clutter).

    So I'm not sure about a portable touch plate. The touch plate feedback needs to go deeper into the control than I have delved as it would need to be set up as an input. It would not be as simple as just setting a value for 3411 unless it shipped with the sensor originally (and then it shouldn't be movable I think). If it shipped with that sensor, it should be wired in to the controller (even if wireless - the receiver should be wired in).

    There is a setting on the panel that forces it to touch off before running that tool - you usually want it off as it takes forever and if you haven't changed the tool its pointless - but you could turn it on and see if the machine goes to a spot and tries (estop at the ready) and if it does then mount the sensor in that location - flat and level - and then set the 3411 variable. I honestly can set tools manually in about 30sec to a minute at most - which is about the same speed as the machine does (as it goes really really slow as it does not know when the new tool might hit the sensor). I have the benefit of eyes and can rapid it to within an inch and mpg it to the table from there. Then a simple minus equation for the z offset and boom its set up.

    In case anyone is wondering, I'm the twin of the other gfacer on cnczone...


  11. #11
    Member
    Join Date
    Aug 2009
    Location
    Canada
    Posts
    655
    Downloads
    0
    Uploads
    0

    Default Re: Spoil Board

    On the crashing bit - you can back up your macros and settings etc. Take the time to figure that out.

    In case anyone is wondering, I'm the twin of the other gfacer on cnczone...


  12. #12
    Registered
    Join Date
    Jun 2017
    Location
    United States
    Posts
    54
    Downloads
    0
    Uploads
    0

    Default Re: Spoil Board

    I am buying it from a cabinet company, its 3 years old and since then the manufacture has "Upgraded" to OSAI controller. They said they no longer have experience with syntec and would not be able to help. They said technically I am not one of there customers until I pay the 3,500 installation fee. But I am not going to do that because they can help me with Syntec anyways. Question: Are the 3 different spindles to be treated as 3 different tools (T1, T2, T3) in Syntec? And in VCarve do I just assign different tools to (Tool 1, 2, 3). Is this the correct way to make VCarve talk to Syntec?



  13. #13
    Member
    Join Date
    Aug 2009
    Location
    Canada
    Posts
    655
    Downloads
    0
    Uploads
    0

    Default Re: Spoil Board

    Ahh - I think they are better than osai but that is another common one on imported machines. Probably the are set up at t1 -t3 but you'll have to confirm that. You'll have to test with vcarve but likely it is OK.

    Let us know once you have the machine in house.

    In case anyone is wondering, I'm the twin of the other gfacer on cnczone...


  14. #14
    Registered
    Join Date
    Jun 2017
    Location
    United States
    Posts
    54
    Downloads
    0
    Uploads
    0

    Default Re: Spoil Board

    Couple more questions:

    1: I understand that I can set and save job coordinates to G54 so that I can use them at a later time. How do I select G54 or others and make the gantry move there prior to running a job?
    2: I see in Syntec that there are G541, G542, G543, ect... Are these just different options that I can save coordinates too?
    2: How often should I back up my macros and settings?

    Sorry about the all the questions but the guy I am buying it from isnt all that familiar either. He hasn't used the machine in over a year. He started up this cabinet business with a partner but the relationship fell apart before the business could take off so they closed their doors. Neither one of them got to run the machine long enough to fully grasp the concept of cnc. I am heading 3 hours to look at it tomorrow and want to have knowledge of my own so I can test out the machines abilities before making a decision.



  15. #15
    Member
    Join Date
    Aug 2009
    Location
    Canada
    Posts
    655
    Downloads
    0
    Uploads
    0

    Default Re: Spoil Board

    I don't save anything to g54, it's just the corner of my spoil board /vacuum grid I think. Same with other g54 options - I don't use them so you'll need to play around. I don't think it's that hard to figure them out.

    Just back them up when you get it and when you're happy with any changes.

    Sent from my LG-D852 using Tapatalk

    In case anyone is wondering, I'm the twin of the other gfacer on cnczone...


  16. #16
    Registered
    Join Date
    Jun 2017
    Location
    United States
    Posts
    54
    Downloads
    0
    Uploads
    0

    Default Re: Spoil Board

    Ok Thanks, I will reach back out to you when I have more questions. Thank you for your time.



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

Spoil Board

Spoil Board