So I'm currently working in speeding up my Holemaking programming time and I'm trying to utilize the feature recognization to help me do this. Keep in mind that I do not own the license to modify and teacher the FBM library so I am limited there.
The way I currently do this is I spot drill all my holes, then drill, counter bore, chamfer, then tap or ream to finish them. I create each operation seperately by (example) Selecting the spot drill operation and selecting all the holes I want spotted and I optimize the tool path for the shortest path. The selection of the holes and there different diameters doesn't matter to me because its just a spot drill, I just like to have a little spot for the drill to follow. Then I repeat this process, making an operation and selecting the holes based on similarities and diameters till the holes are completely finished. With many holes, you could see why this would take a while and why I'd like to make this process easier. The upside this method is I can make very efficient toolpaths.
What I would like to do instead is first, find all my hole features and then group them together based on the vector of my MCS, with I currecntly know how to do. My issue is even after I optimized the tool order selection the actual tool path is not the most efficient. Currently what I'm able to do is insert a spot drill operation for each grouped feature and then optimize the tool selection order but it will sport drill each individual group first before moving onto the next group. Is there a way i could optimize this to create the best tool selection and toolpath? I will include an example utilizing both method to show exactly what I mean. You can see in method_2 the 3 spot drilling operations at the start of it isn't an optimal toolpath. Everything else seems to work fine.
Solved! Go to Solution.
The solution is simple; use the Object -> Optimize command on the METHOD_2 program folder.
Select only the "Create Optimization Group". The result will look like this:
The software will "replace" the 3 individual spot drilling operations with a single "OPTIMIZE_NC" group. Regenerate everything (note that the original spot drilling operations won't need to be regenerated) and review the resulting optimized tool path:
Double click the OPTIMIZED_NC if you would like to use a different sequence of the operations.
I hope that this will meet your expectations.
P.S. I noticed that you are using SOLID_PROFILE_3D for milling the chamfers in METHOD_1. Any reason why you are not using the HOLE_CHAMFER_MILLING operation? Like with the spot drilling operations, you can use Optimized Groups to machine them together in an optimized way even though you program them individually per feature. Have a look at the updated part file.
Tom van 't Erve
NX CAM Development
Nevermind. I remotely accessed my work computer and that worked very well. When I read the Help file for the optimize dialog its a little vague and I didn't understand that this is what an optimization group was. To think I was so close yet so far...