Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.
Showing results for
Show only
|
Search instead for
Did you mean:
This page has been translated for your convenience with an automatic translation service. This is not an official translation and may contain errors and inaccurate translations. Autodesk does not warrant, either expressly or implied, the accuracy, reliability or completeness of the information translated by the machine translation service and will not be liable for damages or losses caused by the trust placed in the translation service.Translate
We are working on generic post processors for the Okuma Multus mill-turn machines. We would be happy to get some feedback from you before we put it into production. Feel free to download and test these post processors and provide any feedback you might have. Thank you. You can download it from the following links.
The "c" has only a main spindle, The "w" has a sub spindle. That's the main difference.
I'll try and see why the XZC is not working on your windows along with the other things you mention. Is that a "Trace" toolpath your trying that is not working in XZC?
Perfect. Thats what i thought and I am using with the W as I have a sub spindle. Yes it is a trace tool path doing a 3d spherical. You should be able to model up something similar easily. About 3" diameter OD and 2.8" ID . 1" x 1.5" Long windows. Roughly as thats the most in depth Im technically allowed to mention. I mill it out using IGF on the Machine as I have IGF set up dang near to be one touch like their name implies. I just cant do 3d chamfering. Trace seems to be the only thing i can get to follow the spherical contours for an even chamfer. Mastercam I can easily pick 2d contour and choose the geometry and it does exactly whats needed to be done converting to a 3d path.
I did a deburring pass on it with 4 axis set so it should give the same results as what your trying to do. The output is TCP mode using G255. Does you machine support TCP mode using G255?
@billcainautodesk Thanks for the file. Which has an Issue. Needs to be sphere for what im looking for. The cylinder a 2d contour, wrapped would work too. But its a sphere that I work with on our parts about 95% of the time.
Also, in the nc post it spits out TD=080001 M323 which is Position 8 on a multus after switching your setup to work on the sub spindle which is where Im doing this currently. If Im coming in perpendicular to the turned part like you should be able to visualize. That should be position 11 or 12 on the sub spindle and 5 or 6 on the main spindle.
For TCP mode the position is correct. Position 1 for the Main, 7 or 8 (Depending on machine option) for the sub spindle. If you position it anywhere else the TCP will not work correctly.
I see the Sphere now. Everything should work the same. Did you still want just 4 axis movement or full 5 axis?
@billcainautodesk The simulation on both of those tools don't look pleasing. edges vary a lot. would produce an uneven chamfer around. Have you worked with a multus at all? I'm just curious, I'm new to it myself but, position 1 the head is tilted 90 degrees like you're trying to drill a hole as a regular lathe! Position 5 and 6 are the proper for spindle 1 and 11 and 12 for the sub spindle. Here is Okuma documentation on what I am talking about. Hopefully this helps us together. I'm needing to come down on the side of the parts, position 5/6 and/or 11/12. Otherwise I don't have a position 1 selected for my tools because its not the position that is needed and doesn't even correspond to what is needing to be done.
Im currently having a post created for our 2 multus b250's and its getting close. i can tell you a couple things in your post that wont work that we've had to change. wherever your post is putting out a G1,G2,G3 the multus will alarm, simply needs to put out G01, G02, or G03. Not a fan of the moves after each operation. Mine posts G21 HP=4, seems more efficient. If you fix these 2 things, ill keep running it through CAS and let you know more differences and try to help you dial this in for people. thanks
@CONNOR_MCDANIEL6Q79R This posts works with the G1,G2,G3. Thats a basic g code about 98% of machines understand with or without the 0. You can edit the post by searching "HP" in the post editor and change the HP=1 to HP=4 and HP=2 to HP=4. It sets one for each spindle which Id like to do the same eventually as the B250 is a tight work envelope.
hmm these multus's wont read the G2's or G3's without being as i mentioned. interesting. im learning a lot about posts lol having one designed for us. its taken a lot of edits so far but like i said its getting there. i will keep my eye on this thread and see if anything comes across it that i can help out with.
So far all I can use is the trace toolpath to chamfer some spherical parts. On my parts not being able to rotate C while using Y axis instead for the chamfers technically makes a skewed 45 degree chamfer which isn't particularly correct. Anyone have a solution yet on the Multus?
We have purchased an Okuma Multus B300IIW, and now we are planning on the CAM side of things. I have a couple of questions on this post.
Are the updated post-processors available where (are these updated to the original post, if any changes has been done)?
Where could I find a machine configuration file for our Okuma Multus B300IIW?
It seems like there is not any difference between OSP-300 an OSP-500 on the Post-processor (we will be having OSP-500)
Is there any differences between metric and imperial system, if we are looking the upload some post-processors or machine config files (we have a metric system in use in Finland)?
The Okuma Multus is currently in Beta stages but the link in this post will always give you the latest version. I am currently working with Okuma and Gosiger in testing and updating the Post so look for some updates coming soon.
There is no machine configuration as of yet because Fusion does not support Turn Mills or lathes just yet. We are working hard on getting the support into Fusion for these machines.
As of now there is only minor differences between the OSP-P300 and the OSP-P500 control. Gosiger has been testing the post on an OSP-P500 control and we have made some changes but they are not ready to be released just yet.
All of our post processors support both metric and imperial systems. While we may make a mistake from time to time we do test both systems to try and catch anything that might have been done wrong.
@billcainautodesk Something else I found may be nice to add is the option for tool groups for tool life management. I have most of my tools set using it using the IGF control programming and it works great but not with the Fusion360 post. Im sure I can manually change it, but being only a chamfer. I'm not too concerned with it cuurently.
@billcainautodesk Just wanted to thank you for the hard work you and team are putting into these posts. This is significantly driving our decision for CAM as you work and we will be testing in parallel as you progress for our B250IIw. I'll be giving feedback soon as we work to test the post on our end.
And good to see there are multiple other users here testing these posts!
@billcainautodesk any updates or knowledge on how to use // usePolarCoordinates - Force Polar coordinates for the next operation (useXZCMode is deprecated but still supported) for the B250 post? Does it only work with specific tool paths?
This was just a name change to clarify what it was forcing the post to do. It is used for milling tool paths and will force it to use polar coordinates (G12.1 in Fanuc). Our posts are typically set to just use XYZ movement when possible so sometimes you want to force it to use Polar Coordinates, and this gives you a way of doing this until we can support that option directly in Fusion.
@billcainautodesk okay thats what i thought. well it doesnt seem to work unless it doesnt work with trace to begin with. I really need this post to prioritize C axis for some operations. I use useXZCmode on my okuma LB3000 and that works great.
