path pilot and fusion

Page 1 of 2 12 LastLast
Results 1 to 20 of 21

Thread: path pilot and fusion

  1. #1
    Member
    Join Date
    Jan 2016
    Posts
    99
    Downloads
    0
    Uploads
    0

    Default path pilot and fusion

    I previously used conversational or g coded what I needed. I'm trying to learn fusion.

    If I use a different size endmill than is programmed with fusion and set it up in the offset page will pathpilot compensate and mill the correct path.

    Thanks
    Dave

    Similar Threads:


  2. #2
    Registered
    Join Date
    Nov 2016
    Location
    United States
    Posts
    151
    Downloads
    0
    Uploads
    0

    Default Re: path pilot and fusion

    Short answer, no.

    First, g-code that uses cutter compensation is different than g-code that doesn't. There are additional g-code commands (G41/G42) and the tool path is different (it is the edge of the cut rather than the tool center), which I guess you already know if you were doing it by hand. Thus, cutter compensation strategies have to start in Fusion (by enabling compensation). Secondly, while some operations in Fusion use cutter compensation, some operations do not, and some portions of an operation might use cutter compensation, and other portions (of the same operation) might not. For example, the roughing part of the operation might not use cutter compensation, while the finish pass of the same operation does. This is fine when the difference between expected and actual tool diameter is a thou or two, but not if we are talking the difference between a 3/8" and 1/2" end mill. In the roughing operation, fusion will not be using a compensation strategy nor issue the compensation g-code commands, and will be driving a 1/2" end mill down a path where it expected a 3/8" end mill. Obviously, it will cut way too much (if not break).

    The point is, even though the strategy you mention might work with something simple and hand coded, it will not work when fusion is doing the g-coding because it uses the compensation strategy only when enabled, only when available, only when needed, and based on the idea that we are talking a thou or two, not a 3/8" end mill versus a 1/2" end mill. Even though what you say is technically possible, Fusion simply doesn't think of "cutter compensation" in the same sense. It thinks of it as something to use at the end of the cut, and expects the end mill be close to the size stated in its tool table, otherwise, during the roughing portion it will have a seriously wrong tool path.

    You can look in fusion and see that compensation is supported in 2D contour, but not in 2D adaptive clearing. It is also supported in 2D pocketing, but it is only used on the finish pass, not the roughing passes. Also note that "enabling" compensation in Fusion means telling it to do it in the controller (on the machine in PathPilot via G41/G42) versus in the computer (internally by Fusion). Technically, you don't enable or disable compensation, you just tell Fusion where to do it. You will see this option on the "Passes" tab where it is available. It is available on most operations, however, as I pointed out above, actually only used on the "finish" portions of the operation.

    One thing I learned about using CAM in Fusion (and I think this applies to all CAM) is to forget about hand coding. I fought it in the beginning, but now I think like Fusion does. You learn the operations and how they work (and their options) and then put them together in a right and efficient order to make the part. There are cases for hand coding an operation as still, but that is not about Fusion. For example, if I need to drill holes very accurately, by keeping all movements in the same direction (to deal with backlash), I might lay that out by hand (or rearrange what Fusion did), but for most (almost all) stuff, I think like Fusion, because that is what I am going to do it in. And I am happier now.


    Quote Originally Posted by toyshop View Post
    I previously used conversational or g coded what I needed. I'm trying to learn fusion.

    If I use a different size endmill than is programmed with fusion and set it up in the offset page will pathpilot compensate and mill the correct path.

    Thanks
    Dave




  3. #3
    Registered
    Join Date
    Nov 2016
    Location
    United States
    Posts
    151
    Downloads
    0
    Uploads
    0

    Default Re: path pilot and fusion

    Btw, just to expand a little bit on learning CAM in fusion. I learned that it isn't as smart as I originally thought. I guess I originally though that Fusion would dissect your design (model) and spit out the necessary operations, with just some minimal guidance. It can't do that. You have to think through the steps in terms of the operations it provides and put them together yourself. It doesn't even know after one operation where the material is left to cut. That is also on you. Thus, since CAM is about you deciding which operations to use, how to use them and in what order to use them, it is necessary that you understand the operations well. When I first started, I was very casual about understanding the operations, because I thought that Fusion did most of that. It really doesn't do much of anything in that regard. What it does do is provide a fairly decent interface (once you become accustomed to it) for setting up each operation, and that is about it. But the details are on you. Once you figure out each operation, you can create a template of it so that you can use it again later, when needed, without having to click through a couple dozen detailed settings. There is a logic to the operations in that you start with a facing op, then an adaptive clearing op, and then pockets or bores or whatever, but it is on you to learn that logic. All fusion will do is execute it (create the g-code). What I did, after fumbling for a couple of months in the beginning, was to focus on each operation and understand it. Create a model with just that operation and play with the settings and make it. And then a couple operations together and so on. Finally, I got to the point of being able to model and cam a complete part with many operations, including multiple setups (flipping the part over, etc.). While I finally understand CAM (at least enough for my needs), I am still surprised how complicated it is. It is still very much like manual milling and thinking through the steps you are going to take, except the that the steps will be done by a machine. Don't get me wrong. The fusion interface is a fairly decent place to select and setup those steps, once you understand it, and you certainly can't do the same steps on a manual mill easily, or at all in many cases, but you do have to understand the steps pretty well. Even something as simple as chamfering will seem complicated until you learn "how" in Fusion. But it isn't too bad. I got my machine in March, and I hadn't done any CNC before that. I kind of delayed moving fully into CAM, cause I thought hand coding would be fine. And I still use conversational when that is all I need. But CAM opens it all up.



  4. #4
    Member
    Join Date
    Jul 2016
    Location
    United States
    Posts
    140
    Downloads
    0
    Uploads
    0

    Default Re: path pilot and fusion

    " It doesn't even know after one operation where the material is left to cut."

    Not exactly true.


    Tormach PCNC 1100 Series 3 w/ Rapid Turn, Fusion 360


  5. #5
    Gold Member daniellyall's Avatar
    Join Date
    Sep 2009
    Location
    New Zealand
    Posts
    1856
    Downloads
    3
    Uploads
    0

    Default Re: path pilot and fusion

    Quote Originally Posted by syscore View Post
    Short answer, no.

    First, g-code that uses cutter compensation is different than g-code that doesn't. There are additional g-code commands (G41/G42) and the tool path is different (it is the edge of the cut rather than the tool center), which I guess you already know if you were doing it by hand. Thus, cutter compensation strategies have to start in Fusion (by enabling compensation). Secondly, while some operations in Fusion use cutter compensation, some operations do not, and some portions of an operation might use cutter compensation, and other portions (of the same operation) might not. For example, the roughing part of the operation might not use cutter compensation, while the finish pass of the same operation does. This is fine when the difference between expected and actual tool diameter is a thou or two, but not if we are talking the difference between a 3/8" and 1/2" end mill. In the roughing operation, fusion will not be using a compensation strategy nor issue the compensation g-code commands, and will be driving a 1/2" end mill down a path where it expected a 3/8" end mill. Obviously, it will cut way too much (if not break).

    Why would you wont cutter comp in a roughing op, you can add in hand coded G Code and macros into fusion

    <img src="https://ivxo1q-dm2305.files.1drv.com/y4mENMmTr_Cabc7pR0FUdB6gtbADq2JbuG4_rGy0eBQvLJx19pTi6TqMUIJN0xgOyDIc0gWoxYhS38HpbSTFGdfaK-o42IOU6jczrhDpfpCOTNGL1X6hvZCbgj0y35gqmq1YGTrWwShYGV-C7lXA2esy0Pi_WfnBSyroDLSGXwce4uSr1U7op7srdi78rispHCa_K4aFlTlJPVkkNWMfgh_Tg?width=60&height=60&cropmode=none" width="60" height="60" />

    Being Disabled is OK CNC is For fuN


  6. #6
    Registered
    Join Date
    Nov 2016
    Location
    United States
    Posts
    151
    Downloads
    0
    Uploads
    0

    Default Re: path pilot and fusion

    Quote Originally Posted by daniellyall View Post
    Why would you wont cutter comp in a roughing op, you can add in hand coded G Code and macros into fusion

    I am not saying you would. I was only answering the OP's question. The point was that Fusion mixes compensation g-code with non-compensation g-code, in the same operation even, so expecting to be able to use a 1/2" end mill in place of a 3/8" end mill and have PathPilot make the necessary path adjustments, after the g-code has already been posted, will not work. Cutter compensation is meant to account for very small differences in tool diameter. Not different sized tools altogether.



  7. #7
    Member
    Join Date
    Jan 2016
    Posts
    99
    Downloads
    0
    Uploads
    0

    Default Re: path pilot and fusion

    Thanks for the responses. I've been running manual machines for 25 years in a maintenance shop. The Tormach is my home machine. All the things I do without thinking much about, now I have to make choices with Fusion or on PathPilot. The number of choices just boggle me sometime. But I am making progress.

    Dave



  8. #8
    Gold Member LeeWay's Avatar
    Join Date
    Jun 2004
    Location
    United States
    Posts
    6618
    Downloads
    2
    Uploads
    0

    Default Re: path pilot and fusion

    Just some suggestions.
    Set up a tool table in Path Pilot. Length offsets only. Keep a notebook of these tool numbers, types, sizes etc. Then when you need to change one, write that change down. Either due to tool breakage or you just need the tool holder for a different tool, different job etc.

    Then in Fusion, set up a standard tool library that you will use.
    There is a Tormach library there already. Select the tools that you will use and you can edit the parameters and tool numbers to match yours.

    Then that huge library is whittled down to only what you use on the Tormach.
    Then each job, you can just select the tools you need from that library.
    Do not use any length offsets in Fusion. All other tool parameters are handled here by the CAM and your tool library.

    That should help you get a good handle on which one does what.

    Lee


  9. #9
    Member mountaindew's Avatar
    Join Date
    Nov 2007
    Location
    earth
    Posts
    2151
    Downloads
    0
    Uploads
    0

    Default Re: path pilot and fusion

    Quote Originally Posted by syscore View Post
    But CAM opens it all up.
    CAM software can be very difficult to learn and even stay proficient at using. I decided early to adopt one system and stick with it. Fusion was in beta at that time so I went with $prutcam and just set down and learned how to get some results, then I built on that for years. After a few late nights setting up standard operations, tools, fixtures and offsets made the software more manageable to use and get results.
    I mentioned this years ago that my Tormach mill running mach was a boat anchor without cam software. Recently I upgraded to new CAD $oftware and wished I had also done this a couple years ago. I was using older methods for drawing models because of years of experience with older software and cost of course. What a mistake that was! New software is so cool to use, if you just let go of old methods and adopt new ways of doing things. I can now draw amazing models in less then an hour that use to take me days.
    Imho try to find software that meets your needs. Make the investment in money and time, then stick with it. In time you skills will improve and make the process much more rewarding and productive.
    If it was easy everyone would do it



  10. #10
    Member kstrauss's Avatar
    Join Date
    Apr 2013
    Location
    Canada
    Posts
    1788
    Downloads
    0
    Uploads
    0

    Default Re: path pilot and fusion

    Which CAD software did you purchase?



  11. #11
    Member
    Join Date
    May 2016
    Location
    United States
    Posts
    138
    Downloads
    0
    Uploads
    0

    Default Re: path pilot and fusion

    Its so easy in Fusion (and most other CAM software I imagine) to just change to the tool diameter you want to use and re-post it. Your feeds and speeds would also change, so not sure you'd want to program for a 1/2" then change to a 3/8" at the machine.

    I also take advantage of their setup sheet, i'll print it out and write on it if I see some things that need tweaking. It also give you Zmin, so you know you are getting your stickout right as well as lots of other good info.



  12. #12
    Member mountaindew's Avatar
    Join Date
    Nov 2007
    Location
    earth
    Posts
    2151
    Downloads
    0
    Uploads
    0

    Default Re: path pilot and fusion

    Quote Originally Posted by kstrauss View Post
    Which CAD software did you purchase?
    I went with IronCAD Inovate that is sold thru Tormach for Tormach owners. The Inovate module Is very limited for being able to dimension and or print anything to paper and or do any 2d drawing. That said it makes drawing very complicated 3d parts and assemblies pretty straight forward. As long as most of your use is output to IGES files for cam software its great if you need any other output your going to have to pay for modules

    After watching a few videos I designed a complete set of parts into a assembly. This drawing took about 8 hours total. Very blocky project but something I had designed before, so I could see the difference. All the parts can be export to use in cam software. My cam software also links to models and if used right makes model updates or changes less error prone and time consuming. A couple more examples that were surprisingly easy to draw compared to my old methods of draw, extrude, sweep, add and subtract !

    path pilot and fusion-ironcad1stdrawing-jpg path pilot and fusion-ironcad2nddrawing-jpgpath pilot and fusion-ironcad3rddrawing-jpg



  13. #13
    Member
    Join Date
    May 2016
    Location
    United States
    Posts
    138
    Downloads
    0
    Uploads
    0

    Default Re: path pilot and fusion

    Not bad!

    I went with Fusion since for me its free, CAM integrated and so many resources out there for info.



  14. #14
    Member mountaindew's Avatar
    Join Date
    Nov 2007
    Location
    earth
    Posts
    2151
    Downloads
    0
    Uploads
    0

    Default Re: path pilot and fusion

    Quote Originally Posted by joshetect View Post
    Not bad!

    I went with Fusion since for me its free, CAM integrated and so many resources out there for info.
    Thanks, I have been drawing most of my life and I still see myself as below average compared to work I see all over the net.

    I was very close to not upgrading cam or cad software and start using fusion because of cost and it is so widely accepted. I just wanted stand alone in the dark no net operation "maybe" software. An old fashion concept these days. Even purchased disk installed software wants to run home to mama every chance it gets to see if its ok to play outside.



  15. #15
    Member
    Join Date
    May 2016
    Location
    United States
    Posts
    138
    Downloads
    0
    Uploads
    0

    Default Re: path pilot and fusion

    Just an FYI Fusion is not online dependent mostly (you can work offline for I think 2 weeks). You can also backup all your files locally. As long as the files you are using are cached you dont need a internet connection to work, the full software is installed on the computer.

    I think their 'cloud based' lingo is a bit miss leading in that aspect



  16. #16
    Member
    Join Date
    Oct 2011
    Location
    Australia
    Posts
    134
    Downloads
    0
    Uploads
    0

    Default Re: path pilot and fusion

    Quote Originally Posted by mountaindew View Post
    CAM software can be very difficult to learn and even stay proficient at using. I decided early to adopt one system and stick with it. Fusion was in beta at that time so I went with $prutcam and just set down and learned how to get some results, then I built on that for years. After a few late nights setting up standard operations, tools, fixtures and offsets made the software more manageable to use and get results.
    I mentioned this years ago that my Tormach mill running mach was a boat anchor without cam software. Recently I upgraded to new CAD $oftware and wished I had also done this a couple years ago. I was using older methods for drawing models because of years of experience with older software and cost of course. What a mistake that was! New software is so cool to use, if you just let go of old methods and adopt new ways of doing things. I can now draw amazing models in less then an hour that use to take me days.
    Imho try to find software that meets your needs. Make the investment in money and time, then stick with it. In time you skills will improve and make the process much more rewarding and productive.
    If it was easy everyone would do it
    Agree partly with your sentiment- in the early days I remember reading your posts and the stuff you were doing with sprutcam, I got know where near as efficient as some of the programming you were doing, but you were very committed and could see that your experience was earned the old fashion way ... with hard work.

    But I got the sh*ts with it big time with the last upgrade as like every other upgrade it just never worked out of the box. Having quite a bit of IT experience and spending 2+ hours trying to get the bastard thing not to constantly error without sucesss I ended up throughing my toys out of the pram.

    In the end I wrote to tormach and got a refund on the upgrade and a trial licence for fusion, after I got bounced around with trying to get support! They were very good about it.

    Now started the massive curve of learning a new CAD/CAM package. Still use rhino for serious cad work as it is quicker when timed constrained. But glad I made the shift, will probably keep the sprutcam around for a while as not confident enough in the 4th axis area to let loose with fusion , and it is still got its issues but the are putting serious development into it. But certainly do agree with the comment if it was easy everyone would do it. 🙂



  17. #17
    Member mountaindew's Avatar
    Join Date
    Nov 2007
    Location
    earth
    Posts
    2151
    Downloads
    0
    Uploads
    0

    Default Re: path pilot and fusion

    Quote Originally Posted by al010964 View Post

    But I got the sh*ts with it big time with the last upgrade as like every other upgrade it just never worked out of the box. Having quite a bit of IT experience and spending 2+ hours trying to get the bastard thing not to constantly error without sucesss I ended up throughing my toys out of the pram.
    This is a problem I have with many programs. Before this last upgrade I decided to start with a new 250 gb ssd. Format and install windows 10 along with all my other bloatware in what I call a clean software stack. "ie house of cards" I expected and had some time consuming problems installing, registering, and setting up both cad and cam programs. Sprutcam expected or wanted previous hidden distro directories for silly stuff like posts and your license that it did not create. Pretty easy to fix with some help from support. Iron cad was a pain because I installed a usb version but had used the download version. The files were not compatible and I ended up uninstalling the usb version and reinstalled the download version "pita" . then register ....... Anyway the drama is over and I have setup pretty well. All the tool libraries and posts are in the right place. graphics drivers, 3d mouse, keyboard shortcuts... ............................all configured Hoping to have a year or so of problem free use. lol



  18. #18
    Member
    Join Date
    Oct 2011
    Location
    Australia
    Posts
    134
    Downloads
    0
    Uploads
    0

    Default Re: path pilot and fusion

    Did the same, fresh install, but windows 7. Had the same licensing issues, which seems crazy now they have gone to a non dongle setup. Really don’t understand why they put this dependence on previous files Into the equation. It should just be a fresh full distro. and it would probably halve the problems. As for the tool library, it has been a root from the start which for me was I think about version 6 and it still does the odd random thing(s) but admittedly far better than what it was day one.

    Touch wood, I haven’t had any of the dramas with the fusion library. They seem to have got it right from early on, sprutcam needs to cut it losses and re-write that module.

    It’s just crazy that you need to spend an hour on the line with tech support to make every version they role out work. I honestly can’t remember one install where it just installed and bang its ready to go, made even worse by the fact I am in oz with no local support so have to call the USA in the middle of the night.

    Anyway end rant

    You mention the 3D mouse ! These things are a god sent I got the space mouse .... only wish I had found them earlier.

    Cheers,
    Adrian



  19. #19
    Member mountaindew's Avatar
    Join Date
    Nov 2007
    Location
    earth
    Posts
    2151
    Downloads
    0
    Uploads
    0

    Default Re: path pilot and fusion

    Quote Originally Posted by al010964 View Post
    . Anyway end rant

    You mention the 3D mouse ! These things are a god sent I got the space mouse .... only wish I had found them earlier.
    Software rants are normal for me anyway. I had to update to windows 10. Windows 7 was old and getting flakey to update and all my other devices in my house run on or are controlled by windows 10. "big house of cards"
    And I couldn't imagine using a 3d cad program without a 3d mouse. Regular mouse on right and 3d mouse on left with keyboard in center and three 25.5" monitors that can be rotated and positioned in portrait or landscape mode for full wrap around effect. I cam simulate left, right, and front views on 3 different monitors sometimes



  20. #20
    Gold Member daniellyall's Avatar
    Join Date
    Sep 2009
    Location
    New Zealand
    Posts
    1856
    Downloads
    3
    Uploads
    0

    Default Re: path pilot and fusion

    <img src="https://ivxo1q-dm2305.files.1drv.com/y4mENMmTr_Cabc7pR0FUdB6gtbADq2JbuG4_rGy0eBQvLJx19pTi6TqMUIJN0xgOyDIc0gWoxYhS38HpbSTFGdfaK-o42IOU6jczrhDpfpCOTNGL1X6hvZCbgj0y35gqmq1YGTrWwShYGV-C7lXA2esy0Pi_WfnBSyroDLSGXwce4uSr1U7op7srdi78rispHCa_K4aFlTlJPVkkNWMfgh_Tg?width=60&height=60&cropmode=none" width="60" height="60" />

    Being Disabled is OK CNC is For fuN


Page 1 of 2 12 LastLast

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

path pilot and fusion

path pilot and fusion