Skip to main content
B
bukaj.lesyk1-Visitor
1-Visitor
February 2, 2011
Question

CAD is OK, but CAM is not a CAM

  • February 2, 2011
  • 21 replies
  • 23814 views

Dear PTC CEO and programers.
Deae PROE FANS

I wrote this to the PTC, but no response.

Forward message>

I am using PROE WF5 PRO/nc as cad/cam system
CAD is OK I like it.
BUT!!! CAM-PRO/NC is not a CAM. When you make something new it is 80% buttons an menus, but engine is the same all the time.You are making olny small changes. Your "CAM" can not compute toolpaths on backround (multitasking)It is not using multiple core technology, I am siting on my chair an waiting for hours. (I have XEON64bit 8GB RAM HP Z400) So wake up PTC. You have a lot of bugs in your "CAM" I am not your employe tester. Bugs are in re-rough, Rough, Finishing, Profile, local mill and surface steps. There are bugs and engine is not good too.
I am using EDGECAM too. If you will sleep, I will throw proe away.(to the recycle bin)

Sorry for my english. It is bad, but it is better then then your "CAM"
You have two options
1.new engine for PRO/NC
2.integrate pro/toolmaker in pro/nc

Bukaj

    21 replies

    Show previous replies
    D
    DanielSantos1-Visitor
    1-Visitor
    February 3, 2011

    Bukaj,

    Talked to a PTC guy today and I need to add a remark to my last statement: If you set your own machine as the remote computation server, then Pro/NC job manager will use the multi-cores you have and it will not attempt to grab another NC license: it will use the license you are using.

    I'm not sure which toolpaths supports multi-core processing or if all them do it. It would be good if someone from PTC could clarify this, an old doubt I have...

    By the way, HSMWork also licenses the NCGraphics kernel, and two ex-NCGraphics employees are now working as freelancers, coding for Cimco/HSMworks... you can find their blog here: <u>www.freesteel.co.uk</u>- Wikipedia says that aproximately 10 CAM vendors licenses NCGraphics technology... so I think Creo/NC will have an interesting future...

    Rgds,

    Daniel

    D
    DanielSantos1-Visitor
    1-Visitor
    February 3, 2011

    Bukaj,

    By the way:

    My last post was not clear, sorry: Pro/NC does not have multi-core toolpaths... it won't split the computation of any toolpath in multi cores... what it will do is to run Pro/NC in one core and compute the toolpath in another...

    HTH

    Daniel

    P
    ptc-19327451-Visitor
    1-Visitor
    February 3, 2011
    No really interesting for my use, I always thought that by using the 'standard' hole features, NC automatically grouped like holes for processing without adding specific NC-based annotations and UDF's to the design model.



    My issue is as follows:



    I machine graphite electrodes for die sinking. I am die designer and do this to help with the NC programmers workload.

    The machining center and tooling package is brought into Pro-E using a standard NC assembly template. I only have options to adjust the overall tool length and flute length of each tool in the package to provide the shortest tool practical.



    I need to do approx 4 standard NC sequences:

    1) volume roughing using a fairly large tool (1.00" bull nosed end mill)

    2) Trajectory finishing of the electrode OD using a similar tool

    3) Semi-finishing of the electrode contour only using an intermediate tool (possibly a 1/2" ball mill)

    4) finishing the contour using a smaller tool (possibly a 1/4" ball mill)



    I have the option to add or subtract NC sequences from this list but these sequences should be able to be brought up from a template of some kind.



    The electrode material is graphite, the sequence / cutting tool should be limited by the following:

    target surface footage of 250 ft/min

    target chip load .003" per tooth

    Max spindle RPM 4000 (yes it is an old machine)

    Max feed rate 40"/min (did I mention that the machine is old?)



    If I choose to change the finishing tool from a 1/4" ball nose mill to a 1/8" ball nose mill (for example) and from 6 flutes to 4 flutes, the speeds and feeds for this sequence must maintain the restrictions listed above.



    Problems with sequences:

    In the scenario above, the machining sequences are as follows:

    1) Volume roughing:

    NC does a good job creating the stock model to use for cutting. I can offset the stock model by about 1/8 inch to allow for rough stock in any direction.

    I have pre-defined sequence parameters in *.mil files for particular combinations of cutting tool, and processing parameters, but these do not update for cutter / cutting conditions automatically.

    2) Trajectory machining:

    I now have to use 'custom trajectory' vs 'trajectory' for a sketch to define the 2D OD profile for cutting. I have to manually define the lead-in and lead-out along with defining the offset side twice, as the system seems to forget the offset direction after exiting the custom trajectory dialog. I use pre-defined *.mil files for this sequence and conditions. Small changes in the model can cause this feature to fail.

    3) Semi-finishing:

    I would like to use (and have used prior to pro-e) 'window' machining to 'lace' across the contour at a prescribed angle but the window-finishing sequence does not allow this. So I have to create a manufacturing surface and then use surface machining to lace across the surface. Again I have pre-defined *.mil parameter files for this. The manufacturing surface is created by seed and boundary, but is prone to failure with minor model changes.

    4) Finishing:

    This works OK. I can create a 'window' to use for machining, set the depth of the window, and then using the 'finishing' sequence options to finish the contour. Using 'Smart retract' often causes the cutter to crash into the model during rapid positioning, so I use retract-always and this creates a lot of redundant retract moves (the retract plane is 3" above the top of the part being machined). I have pre-defined *.mil parameter files for this sequence.



    Now, I have been told (since WF2 or so) that by using the machinability database, I could set up 'seed' values of surface speed and chip load for combinations of materials and cutting types (roughing / finishing) and processes (milling/drilling/turning). This never seemed to work. Also setting up the machinability database directory structure for the cutting tools worked, but caused the *.xml files in this directory structure to be overwritten every time they were used.



    I like the idea that the .xml files can have some intelligence but because of the problems using the .xml tool definitions listed above, I use the older *.mil files. These files have the cutting parameters listed as speed and feed which must be manually compared with the desired surface speed / chip load per tooth as these parameters are not parametric.


    N
    NickMihelich12-Amethyst
    12-Amethyst
    February 17, 2011


    In Reply to Daniel Santos:

    My last post was not clear, sorry: Pro/NC does not have multi-core toolpaths... it won't split the computation of any toolpath in multi cores... what it will do is to run Pro/NC in one core and compute the toolpath in another...

    Hey Daniel

    Is there a better guide to setting up the job manager to process toolpaths on multiple cores? The help files seem to be lacking some details. would there be a diffrence between xp and 7?

    D
    DanielSantos1-Visitor
    1-Visitor
    February 17, 2011
    I don't think there is any difference between XP and 7.

    I can help with a guide. Let me find one here on my stuff... François Lamy created one a few years ago...

    Daniel
    D
    DanielSantos1-Visitor
    1-Visitor
    February 18, 2011
    Nick,

    Please find attached material created by Flamy some years ago.

    First off, you need to install the PTC Distributed Services option in
    the machine you want to serve as the remote computation server.




    Some tips:

    In the machine you want to use as the remote server (It can be your own
    machine), create a batch file calling the Distributed Services
    (dcadsetup -f) manager upon your Windows startup. This will make the
    daemon awake and therefore Pro/E will be able to send the computations
    to the remote server.

    Put this .bat file in the Startup folder so that the script runs
    everytime Windows starts... - Make sure you have the loadpoint\bin &
    \obj folders in your PATH variable so that the .bat script can find the
    files in the loadpoint.

    The dcadsetup is a .bat is a file stored in your loadpoint\bin - It
    also establishes a communication between the job manager daemon &
    pro_comm_msg.exe & the Name Service Daemon (nmsd.exe), the last two are
    solely responsibles for any communication between Pro/E and external
    Apps (Toolkit). Pro/E does not talk directly with other apps... it needs
    to be done through these two guys...

    That said, it might be necessary to edit the two sections of the
    dcadsetup.bat file to match your .bat and .psf files, if you have
    different ones to launch Pro/E with NC license modules.
    If you use your own machine as the remote server, I think it won't be an
    issue... but if you use a remote server, then Pro/E (xtop) will be
    launched as a process, just like in your machine, but it won't show any
    GUI. Anyway, it needs to load the necessary NC licenses, and if these
    are set in specific .psf files (And the .bat associated to them), they
    need to be set here.





    Since Pro/E will be launched to computed the toolpaths (In case the
    server is a different machine), it is important to install the DCAD
    server with the same datecode and release of the client machines. You
    expect to get the same result you'd get at your machine right? So in
    case of an update/upgrade in Pro/E, keep in mind you need to update the
    remote server as well. If you don't, you can get unexpected results.
    (More than the usual ones ;->)

    Hope that helps,

    Best regards,

    Daniel







      H
      hheinze11-Garnet
      11-Garnet
      August 15, 2024

      Wow, thank you. This helped a LOT. I never found out how to find a server. Now I managed it. I just wonder now how I can set that server in a way that I never have to designate that server(s) I want to use again.

      Like setting that server ip / hostname inside a proe-config.

      P
      ptc-19327451-Visitor
      1-Visitor
      February 18, 2011
      When the dcadsetup.bat runs at startup, does it 'grab' a license of NC
      right away, or only when distributed services are requested?

      If it only grabs a license of NC when requested, what happens when one
      is not available?





      Christopher F. Gosnell



      FPD Company

      124 Hidden Valley Road

      McMurray, PA 15317

      PH:724.941-5540

      FX:724.941.8322

      www.fpdcompany.com
      D
      DanielSantos1-Visitor
      1-Visitor
      February 18, 2011
      "of NC right away, or only when distributed services are requested?"

      Only when requested. (If you use a remote server and not the machine
      your running Pro/NC)

      "what happens when one is not available?"

      If you use your machine as the remote server, that will never happen. If
      you use a remote server, the toolpath won't be computed.

      Daniel
      P
      ptc-19327451-Visitor
      1-Visitor
      February 18, 2011
      OK. In my situation, all of the NC licenses are floating, and I 'grab'
      or 'release' a license as needed.



      If I am currently using an NC license, and have my computer setup for
      distributed services on my machine, are you saying that the
      dcadsetup.bat will use my existing activated floating license?

      And while the distributed services are calculating my cl file, will I be
      able to do other tasks in Pro-E? Currently, when a CL file is being
      calculated locally, the software is 'busy' and unresponsive.



      Thanks for taking the time to explain this feature; I don't mean to take
      up so much of your time,





      Christopher F. Gosnell



      FPD Company

      124 Hidden Valley Road

      McMurray, PA 15317

      PH:724.941-5540

      FX:724.941.8322

      www.fpdcompany.com
      D
      DanielSantos1-Visitor
      1-Visitor
      February 18, 2011
      "If I am currently using an NC license, and have my computer setup for
      distributed services on my machine, are you saying that the
      dcadsetup.bat will use my existing activated floating license?"



      Yes.



      "And while the distributed services are calculating my cl file, will I
      be able to do other tasks in Pro-E? Currently, when a CL file is being
      calculated locally, the software is 'busy' and unresponsive."



      That's the best part of it. You wil be free to create new toolpaths...
      great for mold makers.. that are used to long computation times...



      Pro/NC was very innovative on this... it's pity that they could not keep
      ahead of the competition... with things like that, they were, 10-15
      years ago...



      Daniel

      Show more replies
      Terms & ConditionsAccessibility statement