Tool path efficiency questions

This is the main step of a part we produce. Currently it takes 9+ minutes to run this code through the rough, finish, & flatlands operations. I don't have a lot of experience with machining using the 3-axis, usually for our needs 2-axis has always been sufficient.

I did try the advance rough with no time benefit. It just seems like doing this small of a part should be faster.

Would like if someone fluent with BC would mind taking a look and see if they see efficiency improvements I could make?

Just in case the EM's dont transfer with a bbcd file, I am using a 3F .5 carbide and a 3F .1875 carbide.

I am running V26
Part is being run on a HAAS Mini
6k spindle

Thanks

how many parts ?
tolerances,any critical ?
surface finish ?


You have to consider how much programming time is acceptable VS. quantity and or quality of part

If a guy was to take his time with the CAM and do the part in all or mostly in 2D paths in a planned and logical way,you could beat that time,,actually by a lot,,,IMO,,
programming time will be longer.CAM tree will be a lot bigger,You get a lot more control,,,,,my .02 cents

2-axis has always been sufficient.

yup,usually is for me too

Thanks for the reply.

Quantity is several hundred+
Tolerances would be +/-.005
Finish is tumbled in plastic/abrasive pyramids to remove burrs and tools path marks.

I thought of doing it 2-axis but, this is a 4 step assembly line type fixture, although the other sides are simple and fast engraving and drill holes, etc. I was afraid of losing the "consistency" for lack of better word. Meaning, this is my shape and as a 3-axis I know it will be the same each time. With 2-axis it seems like I lose that control although I know its a mental thing. I guess its just not being able to see the block anymore and just seeing rectangles used for pockets.

Whether you use 2d or 3d toolpath strategies, it really comes down to physics in the end. There is "X" amount of material to remove with "X" amount of machine/tool capability. Some minor efficiency gains can be found, and given that this is a relatively low tolerance part I think you can expect better than 9 minutes, but that also depends a lot on your machine and whether or not the tools you specified in your Bobcad file can perform as needed.

One thing to keep in mind is that the adaptive toolpath strategies like Advanced Rough offer most of their efficiency through deeper passes and smaller step overs at higher feeds. Standard strategies step over more and cut more depths, which adaptive strategies are meant to work the other way around. The trick is to find a depth of cut that squeezes into the steps of your model. In this case, you have three depths that need to be roughed out in the first op, so finding a depth of cut spacing that gets all three as close to the part surfaces as possible is a little bit of trial and error. It is a roughing pass though, so you only have to get it to a manageable remaining stock for the subsequent passes with a smaller tool. With +/-.005" tolerances, I would then follow up the first Advanced Rough with a second Advanced Rough using "Rest Machining" and the smaller bit, as well as no allowance. You can clean up the part to the point of being nearly finished with that operation. After that, I'd go with a "Flatlands" operation and set the minimum size of the flatlands to a small amount so you catch all of them, again with the smaller tool.

This method will not be the cleanest part, but I would venture to guess it will meet the tolerances you spec'd. If you want a smoother finish off the machine, it should be obvious that "more time" = "better finish". If the priority is speed, this would shave it down to perhaps 7 minutes or less depending on your machine rapids and acceleration. I don't think you're going to get any faster unless you have a more capable machine. I can run about double the feedrates, but I also can spin the bits up to 15,000 rpms.

I've attached a quick example of how I'd approach it with the specs you gave, but there are a few places where I might add a quick 2d geometry to rough out some stock the automated strategy missed between the first and second ops. I don't like seeing a bit go full width on cuts, so anywhere I see that I might split the strategies up and add in a 2d manual roughing pass in very specific areas. Didn't take the time to do it here, but you could do so pretty easily. You'll see what I mean as there are a couple spots where the smaller bit goes through the material full width. I did not change the feeds/speeds from the standard settings, but I might do so if I thought the bits could take it. Or, you could also try a bigger step over, but IMHO it's better to increase feedrate and take smaller stepovers as the first option. Really depends on your machine's specific traits.

Thanks for taking the time to explain all that as well as attaching the file. One thing I did notice is even when using your file after dropping the speeds and feeds down to a number my machine is capable of I was right back at the 9+ min mark. As you stated I am having to run the .1875 bit slower feed than I'd like because of a few full width passes as well as some inside corners.