5 axis - Machine Simulation Software, Absolutely Necessary? Or "She'll be right"?
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 39
  1. #1
    Join Date
    Jul 2021
    Country
    AUSTRALIA
    Posts
    16
    Post Thanks / Like
    Likes (Given)
    24
    Likes (Received)
    13

    Default 5 axis - Machine Simulation Software, Absolutely Necessary? Or "She'll be right"?

    Hi Cuties,

    In anticipation of taking delivery of our DMU75 in February, armed with nothing but basic YouTube knowledge, I have begun fantasizing about all the different ways I am going to completely bin the brand new machine. Rapid the spindle into the work piece? Maybe a nice table to spindle crash?

    In order to prevent* this from happening I have been advised by the shops we went to visit, who are running these machines, that it's a good idea to get a 3rd party simulation software to verify that the G-Code being posted (we will be using Master Cam) isn't going to hinder my ongoing employment.


    We are look at the Vericut software as that's what was recommended to us - it's worth $47,000, that's $34,500 in freedom coins, that along with the $50g (aus) price tag on the CAM software package which I understand is unavoidable, has all added up very quickly.

    The guy that is supplying the software packages has alluded to that the CAM has a capable crash detection element to the software that could be implemented which would allow us to potentially get away with not having the 3rd party software, but seeing as a spindle is worth 30k it only has to work twice to pay for itself... right?


    What do you guys think? Is it something we could get down the line, or is it a must have from the get-go? Also, what other platforms are people using? What else could/should I be looking into?

    All options, opinions and venomous/witty remarks are more than appreciated.

  2. #2
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    1,552
    Post Thanks / Like
    Likes (Given)
    233
    Likes (Received)
    978

    Default

    We use master cam with post ability it was 7k for simulation it works pretty good for the money
    Don


    Sent from my iPhone using Tapatalk Pro

  3. Likes goooose liked this post
  4. #3
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    2,262
    Post Thanks / Like
    Likes (Given)
    941
    Likes (Received)
    2939

    Default

    First, that quote for Vericut is absurd.

    You can buy a seat of NX CAD + 5 Axis CAM + NX Simulation for less than what the dindgongs at Vericut want for simulation only. NX is the best CAD (hands down), better CAM than MasterCAM, and the fact that you run the simulation inside of one package saves tremendous time and headaches. Not only is NX cheaper than the tool chain you're looking at, it is more capable and the complete integration between everything takes it all to another level.

    But, as to your original question - every CAM package out there has a simulation function that animates what the tool path and material removal will look like. The trick is; this simulation is being driven by the CAM system's internal tool path and has no connection to how your machine is configured. I cannot speak for MasterCAM, but both Fusion (the very low end) and NX (the very high end) have such solid internal simulation that I think someone with some machining experience could be comfortable relying on it to trust code.

    One trick folks use is to define the tool holders with the taper section (which is irrelevant to simulation anyhow) being modeled to the full spindle head. If you combine this with CAM setups featuring the full table and work holding, you generally can be very confident in the code you are posting.

    The trick to all of this, is that you need to test the heck out of your post-processor and (if you have G-code simulation) your machine simulation setup. If you think of it, we have a post processor that is translating the CAM's internal toolpath into G-code for your machine. If we simulate that G-code, we need a machine kit that tells the verification software exactly how your machine operates - a kinematic model, control configuration, and code treatment. Any way you slice it, you'll be creating test programs and running them on the machine (often with no tool or work holding at first) just to make sure the code jives with reality.

    What I would do is buy NX instead of the toolchain your looking at. Barring that... I would get the machine, get your CAM, have your purchase order for Master CAM put the vendor on the hook for a 100% perfect post processor for your DMU. When they deliver it, run sample code that goes through literally everything - how the machine retracts between operations, drilling/tapping cycles, tool center-point control/dynamic work offsets/TRAORI, probing cycles... Literally everything. Test 100% of the functions of that post processor before you sign off on anything.

    At that point, you'll have a dialed-in post processor and you'll have some experience very cautiously making CAM programs, simulating them, and posting code. You should have just enough data under your belt to evaluate if a G-Code simulator is actually necessary. If MasterCAM's basic visual toolpath simulation 100% matches what happens on the machine, and you have your workholding and spindle modeled in your libraries? Why spend the money on G-Code simulation?

  5. Likes empwoer, 2outof3, Lukas D, aarongough, Milacron liked this post
  6. #4
    Join Date
    Aug 2006
    Location
    Wisconsin
    Posts
    1,778
    Post Thanks / Like
    Likes (Given)
    810
    Likes (Received)
    836

    Default

    This has always been a topic every time we purchased a 5x machine. We use Powermill to drive our 5 axis machines. IF you set up the machine properly and use the provided collision checking tools, it is rock solid, has been for the 25 plus years I have been using it. We have had allot of simulation demos including Vericut. I had an axis reversal many years back that gave me grief that I did not catch, and Vericut was the only software that actually saw the error. Having said that we still run with no 3rd party software. We almost pulled the plug on CamPlete, but that does not check existing g-code, it creates it's own. Be careful shopping around, some don't actually check YOUR program, (Vericut does). FYI I know several shops that have Vericut and don't even use it, much to time consuming they claim.

  7. #5
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    2,114
    Post Thanks / Like
    Likes (Given)
    2893
    Likes (Received)
    1517

    Default

    Vericut has a "single platform" option for around $11k, that's locked to a single machine definition. That's what I used with my first 5 axis, and it served me very well.

  8. #6
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    6,147
    Post Thanks / Like
    Likes (Given)
    5757
    Likes (Received)
    3928

    Default

    It's definitely not mandatory as we don't have it.
    I use the verification in Mastercam and for what we do it's served us well.

    I can certainly see the justification for it so if you have the budget, then absolutely buy it.

  9. Likes metalmadness liked this post
  10. #7
    Join Date
    Nov 2015
    Country
    UNITED STATES
    State/Province
    Colorado
    Posts
    540
    Post Thanks / Like
    Likes (Given)
    112
    Likes (Received)
    310

    Default

    I went through a very similar buying process back when getting into multiaxis machining. Any shop I have toured locally runs Vericut on their multiaxis machines. The reason is simple - like you say, a spindle can cost $30K to repair/replace if you crash the machine. How expensive is a crash? Very expensive, plus the other hidden costs like machine downtime and loss of revenue. Simply can't afford to have the downtime.

    How expensive is verification software? Expensive, but not very expensive like a big crash. Luckily you won't run into downtime issues with machine simulation.

    DMU 75 is an expensive machine tool. I have had my multiaxis machine for 4 years now. It has never been crashed. I did have a small bump that broke a small diameter tool because of a known plane issue within Mastercam, but I was running 3+2 and didn't use Vericut for that project. IF I hadn't been standing at the machine, my spindle would have smashed into the trunnion because it was aiming for a negative Z value which was through the trunnion. That is going to be a very expensive fix!

    Do I run Vericut for every project? Not really always, especially if I am not running 5-axis toolpaths that are generating a lot of crazy motion or close-calls so to speak. But anytime something big or serious needs running, I am absolutely verifying that.

    As far as the people saying "using Vericut is too time consuming" are being disingenous. It's called using setup templates. If you have 5 main types of fixture setups, create a Vericut environment template for each one. That way, you simply run the Vericut Mastercam Add-in, it opens Vericut, you setup your NC file, find your G54,G55, etc and boom press RUN. That is IT. That is the most basic level of running Vericut...you can sure as hell get a lot more detailed with it if you want to, like using their Force module for adaptive feedrate calcs and stuff. But for basic machine simulation, it is very easy to setup once you've got the hang of it.

    Someone else said NX, first off fuck that. NX is overkill in a lot of regards. Do you need a full PLM solution? NX is what you need. If not, I would say consider Mastercam and Vericut. They play well together. If you run the Mastercam interface for Vericut, your tools and holders are defined within Mastercam so you don't need to sit there in Vericut and create a bunch of redundant holders and tools.

    Another benefit of running Vericut - you can feel confident in pressing the big green GO button on the machine. "I have run this through WYSIWYG machsim and I know that nothing is going to happen" is a really priceless feeling. You can feel okay handing the program off to an operator without standing there proofing it out. Additionally, sometimes with complex multiaxis work it helps to be able to slap a rough toolpath into machine simulation to see how the machine will behave. A lot of times, Mastercam (or any CAM) doesn't do a very good job of showing the programmer how the machine will behave. Vericut running actual posted code will show exactly what the machine will do. It helps tweaking and dialing in complex operations without wasting time cutting air.

    As far as post processors go, you'll need one that you can rely on. I am sure the DMU has a well developed and robust post processor out there, but I would say you should purchase a custom post processor. It is a critical tool in the CAM-CNC chain, and Vericut is only going to show you posted code, so the better that your posted code is, the better results Vericut will give.

    Is full simulation 100% necessary? Not at all. I am sure there are a ton of shops out there that do not run full simulation and use complex machine tools. That's awesome but I am not comfortable putting a $500,000 asset at risk if there is an off the shelf solution that completely negates that risk! One thing to keep in mind is that if you're investing in full simulation, you want to make sure that whatever software you choose is running fully post-processed NC code - CAMplete works as the post and the simulator. NCSimul and Vericut are running posted code. Not sure what NX does. If it is running NCI code then you might miss things like axis unwinds or axis reversals that can really ruin your day. Simulating unposted code isn't going to give you the same level of assurance.

    EDIT: your full quote price does sound very expensive. More like $20-30K plus control building costs should be the actual price unless things have radically changed in the past few yeasr.

  11. Likes DouglasJRizzo, mhajicek, Lukas D, Milacron liked this post
  12. #8
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    880
    Post Thanks / Like
    Likes (Given)
    270
    Likes (Received)
    679

    Default

    I completely agree that you would be better off spending the money on good software and the appropriate post/simulation for that software instead of Vericut.

    Honestly, I only see Vericut as a necessity if you are programming with MasterCAM. It's a tool to catch things that don't show up due to sketchy simulation or sketchy posting.

    Shops using NX, Esprit, Powermill, hyperMILL, etc... almost never have additional simulation. That's what the CAM software is supposed to do. The DMU75 is nothing special. There will be a dozen bulletproof solutions right off the shelf. You don't need to backplot code when the post is well integrated with the machine tool.


    If we were talking about a custom built gantry with a nutating head - then by all means, you should really think about VERICUT. But if your software can't confidently handle posting to a mass produced table/table fixe axis, you need to either ditch the software or fix the issues.

  13. Likes empwoer, CNC Hacker, 5 axis Fidia guy liked this post
  14. #9
    Join Date
    Sep 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    1,402
    Post Thanks / Like
    Likes (Given)
    2191
    Likes (Received)
    769

    Default

    Quote Originally Posted by metalmadness View Post
    I went through a very similar buying process back when getting into multiaxis machining. Any shop I have toured locally runs Vericut on their multiaxis machines. The reason is simple - like you say, a spindle can cost $30K to repair/replace if you crash the machine. How expensive is a crash? Very expensive, plus the other hidden costs like machine downtime and loss of revenue. Simply can't afford to have the downtime.

    How expensive is verification software? Expensive, but not very expensive like a big crash. Luckily you won't run into downtime issues with machine simulation.

    DMU 75 is an expensive machine tool. I have had my multiaxis machine for 4 years now. It has never been crashed. I did have a small bump that broke a small diameter tool because of a known plane issue within Mastercam, but I was running 3+2 and didn't use Vericut for that project. IF I hadn't been standing at the machine, my spindle would have smashed into the trunnion because it was aiming for a negative Z value which was through the trunnion. That is going to be a very expensive fix!

    Do I run Vericut for every project? Not really always, especially if I am not running 5-axis toolpaths that are generating a lot of crazy motion or close-calls so to speak. But anytime something big or serious needs running, I am absolutely verifying that.

    As far as the people saying "using Vericut is too time consuming" are being disingenous. It's called using setup templates. If you have 5 main types of fixture setups, create a Vericut environment template for each one. That way, you simply run the Vericut Mastercam Add-in, it opens Vericut, you setup your NC file, find your G54,G55, etc and boom press RUN. That is IT. That is the most basic level of running Vericut...you can sure as hell get a lot more detailed with it if you want to, like using their Force module for adaptive feedrate calcs and stuff. But for basic machine simulation, it is very easy to setup once you've got the hang of it.

    Someone else said NX, first off fuck that. NX is overkill in a lot of regards. Do you need a full PLM solution? NX is what you need. If not, I would say consider Mastercam and Vericut. They play well together. If you run the Mastercam interface for Vericut, your tools and holders are defined within Mastercam so you don't need to sit there in Vericut and create a bunch of redundant holders and tools.

    Another benefit of running Vericut - you can feel confident in pressing the big green GO button on the machine. "I have run this through WYSIWYG machsim and I know that nothing is going to happen" is a really priceless feeling. You can feel okay handing the program off to an operator without standing there proofing it out. Additionally, sometimes with complex multiaxis work it helps to be able to slap a rough toolpath into machine simulation to see how the machine will behave. A lot of times, Mastercam (or any CAM) doesn't do a very good job of showing the programmer how the machine will behave. Vericut running actual posted code will show exactly what the machine will do. It helps tweaking and dialing in complex operations without wasting time cutting air.

    As far as post processors go, you'll need one that you can rely on. I am sure the DMU has a well developed and robust post processor out there, but I would say you should purchase a custom post processor. It is a critical tool in the CAM-CNC chain, and Vericut is only going to show you posted code, so the better that your posted code is, the better results Vericut will give.

    Is full simulation 100% necessary? Not at all. I am sure there are a ton of shops out there that do not run full simulation and use complex machine tools. That's awesome but I am not comfortable putting a $500,000 asset at risk if there is an off the shelf solution that completely negates that risk! One thing to keep in mind is that if you're investing in full simulation, you want to make sure that whatever software you choose is running fully post-processed NC code - CAMplete works as the post and the simulator. NCSimul and Vericut are running posted code. Not sure what NX does. If it is running NCI code then you might miss things like axis unwinds or axis reversals that can really ruin your day. Simulating unposted code isn't going to give you the same level of assurance.

    EDIT: your full quote price does sound very expensive. More like $20-30K plus control building costs should be the actual price unless things have radically changed in the past few yeasr.
    how in the hell are you gonna say that NX is overkill when you say 20-30k for vericut plus double that for mastercam 5 axis setup? when NX with machine sim is 35k WITH a custom post processor?

    NX simulates actual G code fyi.

  15. Likes boosted liked this post
  16. #10
    Join Date
    Aug 2012
    Location
    Pittsburg, KS
    Posts
    1,366
    Post Thanks / Like
    Likes (Given)
    189
    Likes (Received)
    614

    Default

    I am behind the times as the last 5 axis I had my hands on was from '04-'11. It was a nutating head cnc router. We used Mastercam, no 3rd party sim software. I got very comfortable with it and did some very weird one off projects on it that I had to use all my smarts to make happen. Anyway, the trust I had with our setup was built on the MTB providing us a bulletproof post and I got some very good training on both the machine and MC. So for me I felt like I did not really need something like Vericut.

  17. #11
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    2,114
    Post Thanks / Like
    Likes (Given)
    2893
    Likes (Received)
    1517

    Default

    I think in summary, one can say that if your CAM simulation is dialled, and/or if the programmer is very experienced and meticulous, you can skip it. Otherwise, it's a gamble.

  18. #12
    Join Date
    Nov 2007
    Location
    canada
    Posts
    816
    Post Thanks / Like
    Likes (Given)
    111
    Likes (Received)
    488

    Default

    If you already run and know Mastercam and want to make your life easy, as mentioned above, just get a post with simulation from Postability. You'll need a post anyways so going this route you're already half way there. Postability's posts are tied into machsim so the motion will match that of the machine.

  19. #13
    Join Date
    Nov 2015
    Country
    UNITED STATES
    State/Province
    Colorado
    Posts
    540
    Post Thanks / Like
    Likes (Given)
    112
    Likes (Received)
    310

    Default

    Quote Originally Posted by empwoer View Post
    how in the hell are you gonna say that NX is overkill when you say 20-30k for vericut plus double that for mastercam 5 axis setup? when NX with machine sim is 35k WITH a custom post processor?

    NX simulates actual G code fyi.
    I didn't mean "overkill" in terms of price, i meant overkill in terms of features and functionality. NX is a massive program that probably has a bunch of random things that OP doesn't need for a programming environment. It is a beast of a program and considered to have quite a steep learning curve...

  20. Likes mhajicek liked this post
  21. #14
    Join Date
    Nov 2015
    Country
    UNITED STATES
    State/Province
    Colorado
    Posts
    540
    Post Thanks / Like
    Likes (Given)
    112
    Likes (Received)
    310

    Default

    Quote Originally Posted by goooose View Post
    If you already run and know Mastercam and want to make your life easy, as mentioned above, just get a post with simulation from Postability. You'll need a post anyways so going this route you're already half way there. Postability's posts are tied into machsim so the motion will match that of the machine.
    Dont you have to pay extra to get the Postability post linked to the MachSim environment? I'm guessing it isn't anywhere near as spendy as Vericut but it is a cost to consider.

  22. #15
    Join Date
    Sep 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    1,402
    Post Thanks / Like
    Likes (Given)
    2191
    Likes (Received)
    769

    Default

    Quote Originally Posted by metalmadness View Post
    I didn't mean "overkill" in terms of price, i meant overkill in terms of features and functionality. NX is a massive program that probably has a bunch of random things that OP doesn't need for a programming environment. It is a beast of a program and considered to have quite a steep learning curve...
    of course it has a bunch of things, doesnt mean you have to use them all. with the right VAR supporting you, setting up templates for you, its not nearly as bad as most people think.

  23. #16
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    5,364
    Post Thanks / Like
    Likes (Given)
    1193
    Likes (Received)
    658

    Default

    Quote Originally Posted by goooose View Post
    If you already run and know Mastercam and want to make your life easy, as mentioned above, just get a post with simulation from Postability. You'll need a post anyways so going this route you're already half way there. Postability's posts are tied into machsim so the motion will match that of the machine.
    This is a great option.
    Providing the machine parameters are configured and behave as expected.
    But this also goes for vericut....if the cnc machine doesn't match the Vericut (or NCSimul etc) file, then all bets are off!

  24. #17
    Join Date
    Feb 2014
    Location
    FL
    Posts
    4,588
    Post Thanks / Like
    Likes (Given)
    13938
    Likes (Received)
    5604

    Default

    "She'll be right"... Tell me you're from Australia without saying it in words

  25. Likes Lukas D liked this post
  26. #18
    Join Date
    Jun 2006
    Location
    Near Seattle
    Posts
    5,345
    Post Thanks / Like
    Likes (Given)
    3988
    Likes (Received)
    1656

    Default

    here's a bucket of ice water on the topic....

    any simulation, in the CAM, in something like vericut or ncsimul or whatever, is only as accurate as its model of the machine, and in particular, must make assumptions about what the machine controller will actually do with any particular instruction sequence.

    I once had a circumstance where I made a CAM error, which the CAM/Post magnified by posting wrong code (so we have wrong code for the wrong command), and the controller mis-executed this wrong code. This was quite a headache to sort out.

    which controller will be on your DMU? The Heidenhain in my experience is pretty good at defending the machine, and DMGs may still come with DCM enabled - which is a kind of simluation in the controller. (but DCM, at least circa 2006, didn't know about fixtures, and so it wouldn't prevent crunching a probe body on the end of a vise. you don't have to wonder how I know this.)

    So begin by checking out what controller, collision prevention (and limitations), and "shock defense" will be on the machine.

    And then make sure your simulation solution, be it CAM sim, CAM machine sim, some external simulator - have an ACCURATE model of the machine, the tools, the fixtures, and so forth.

  27. Likes empwoer, metalmadness liked this post
  28. #19
    Join Date
    Aug 2006
    Location
    Wisconsin
    Posts
    1,778
    Post Thanks / Like
    Likes (Given)
    810
    Likes (Received)
    836

    Default

    The last sentence of the above post is an important one. Read it again. Just because you run your toolpath thru Vericut, does not mean everything will be perfect. Some knucklehead could flop a mold core on my magnet 1/4 inch off position and run the verification with a .05 collision distance and it's not going to do a whole lot of good now will it.

  29. Likes bryan_machine, boosted, Milacron liked this post
  30. #20
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    880
    Post Thanks / Like
    Likes (Given)
    270
    Likes (Received)
    679

    Default

    Quote Originally Posted by 5 axis Fidia guy View Post
    Some knucklehead could flop a mold core on my magnet 1/4 inch off position and run the verification with a .05 collision distance and it's not going to do a whole lot of good now will it.
    Yup. It's also not going to catch when the tool holder model you download off machining cloud is missing a .025in dimple on the profile, or when the vise is .125in off center and causes the head to dip into the table when C axis is rotating.

    I programmed for a while in an environment that forced everyone to use Vericut. Had a bad program crash a machine once. Set it up wrong in CAM, then set it up wrong in Vericut. Made it through both of those systems no problem, then promptly punched a hole in the table.

    Vericut is really just a tool for double checking posted code. But in the year 2021, there's no reason for a simple five axis post to be suspect.

  31. Likes CNC Hacker liked this post

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
  •