Thanks again for your helpful suggestions. I'll try all your recepies tomorrow and send feedback on the result.
From what I remember, I've used IPW, and that could be the problem. We'll see what I can resolve tomorrow.
Thanks a lot,
Okay, thanks. I am confident that the Use 3D IPW option is causing the issue. It's basically "overthinking" and "overcompensating". Also, definitely look at the Guiding Curves Drive Method. I have created a video that touches on this. I've provided a link below. Guiding Curves content starts around 18:45, but I encourage you to check out all of the video.
I tried all your solutions. But time has been tight, have got something that I can live with for now. An image is below. I think that this would work with the geometry of yesterday as well, but during the night, I had moved the design to SolidEdge 2019, deleted the original round, and redid the round using offset curves and sweep. That made a reasonably good surface to base the guide curves and streamlines on.
Then I did the guide curve using a ball mill since guide curve does not work with bullnose. I disabled the collision checking and got a +ZM based tool path, then I did the tool path tilt for collision avoidance and with the right parameters it looks gorgeous.
It will be machined on Monday. But I've made a simulation video, and I'll upload it for you to view in a few hours.
Thanks to you all.
Here is the tool path with guide curves with tool tilt. I'm planning on putting this on the machine tomorrow. The actual simulation is somewhere half way in the video. The tool holder is a rego-fix powrgrip, PG10 with a 4mm dia ball milling cutter with a 6mm shank mounted on it.
I am happy the Guiding Curves worked well for you. I assume that for tilting the tool axis you used the avoidance and smoothing option inside the operation and did not activate it from the ONT. correct?
looking on the geometry and tool you are using wonder how you intended to use a bull nose tool. is it really better? we are working to enhance the Guiding Curves to support non ball tools and I want to capture the use cases where this is mandatory.
BTW - if you still need to support the bull nose tool (in streamline) - I would go to the drive method dialog and preview the result there. if it needs refinment - you can do it from that dialog. check between tool on / tanto / contact. After you close it make sure that the Tool Axis orientation is correct and the projection is toward drive with appropriate backoff distance. in 12.0.2 you can youe the projection preview to see where the projection starts and where it is heading.
Another experiment you can do with exporting the Guiding Curves path to CLS and importing it back to a variable axis surface contour operation with tool path drive. if the tool you will be using is a bull nose with the same diameter (and similar shank) - this may provide a nice path.
Good luck in the cutting test
Hello Eddy @Eddy_Finaro
Thanks for your response. Yes, the guiding curves worked well. However, if you see that image, the floor is nearly planar, albeit tilted along the rail of the round. I was planning on a bull nose cutter with CR=1 where the round is R=2. That would still be a safer tool path as the tool will not dig into the edge. So a bull nose with tool axis perpendicular to the floor would've been ideal with 4-5 swarf type tool paths along the round. Thats the reason I was trying to put the streamlines along the round. However, time was tight and I needed an answer. The guiding curves works, but it is also a tool path with significantly larger engagement and thus the potential of vibration. The regofix tool holder with a short tool should be able to take care of it. It would be great if the guiding curves supported a bull nose as well.
I don't know what is ONT? The way I've done it is the following: I did the guiding curves with the tool axis straight along +ZM. Then I right clicked on the operation, and chose Tool Path->Tilt Tool Axis with the following settings.
Ok, so the usecase where this would be manadatory would be closely related to work we do. This is a jig for a forged part. The forgings have a straight edge with a 5deg Relief. This is what would be inappropriate with a ball cutter, since its a 10sec tool path and with a ball mill it will become a 5minute tool path.
The other thing that I found difficult to accomplish was to clean the quality of streamline tool path. I'm very new to NX, so I'm not that familiar with all the tweaks that can be done to clean it up. I'll try your suggestions.
Thanks a lot,
ONT = Operation Navigator Tool
I.e. the listing of the operations/tools/methods/geometry
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled
ROFL, thats exactly what I've used! But I stillhave an issue with the outside edges, I'm getting too close with the C table and Z axis. Let me show what I mean... will upload a video shortly.