Roughing and finishing programing question

[maverickx50]

I often need to do more than one rough cut to reduce machine cutting time. ie .50 end mill then .25 end mill then .375 ball end cutter followed by a finishing pass with maybe a ¼ or 3/8” ball end mill. How do I get each roughing then finishing pass to adjust for what was already removed to reduce unneeded air cutting time?

Thanks......

[gc3]

I often need to do more than one rough cut to reduce machine cutting time. ie .50 end mill then .25 end mill then .375 ball end cutter followed by a finishing pass with maybe a ¼ or 3/8” ball end mill. How do I get each roughing then finishing pass to adjust for what was already removed to reduce unneeded air cutting time?

Thanks......

weird strategy...but hover the mouse over the machined areas to see the -z depth...

[maverickx50]

weird strategy...but hover the mouse over the machined areas to see the -z depth...

Not that strange. A 10" X 10" square 3d shape maybe 5/8" deep may take 8 hours to cut with a 3/16" ball end-mill. By attacking it with first a 5/8" End mill then a 1/4" end mill and finishing up with a 3/16" I can reduce my total cutting time to less than 2 hours. Not counting the 2 extra tool changes of course. But I have extra collets & collet nuts etc so can have them and a next cut tool ready to go with little lost time. Now if I can take the air cutting out of the equation I'll save another 30 min or more.

The Z depth is not the answer as the smaller cutting tool comes with cut depth per pass limits built into the equation. I'd still be cutting a lot of air at the top of the 3D image is usually pretty close to the top of the material zero

[knight_toolworks]

I don't see a need for 3 bits for most 3d jobs. if you do a good roughing pass. what I do is make a few passes in 3d at a slow speed then stop and start the file again at a much faster speed then the bit is only taking off a tiny amount in a pass. or maybe I am missing something? If you did the 3d in a bigger bit then do it in the small one a couple hundreds deeper.

[pkirby]

I'm not sure if it's possible to do what you want in Aspire, but other CAM systems do have this option. It's called REST machining (I think it stands for remaining stock). I own both Aspire and SolidCAM and I find that SolidCAM gives me a LOT more options for 3d machining. It has multiple options for creating work boundaries, and it also has several different machining stratagies instead of just offset or raster. I also find that SolidCAM results in a smoother surface finish because Aspire is pixel based which can result in jagged edges on steep surfaces. I've talked with Aspire about it and they gave me some tips on increasing the model resolution in the job setup menu but that still didn't completely help. Below are 2 screenshots of the exact same file that was created in Rhino but one was imported into Aspire and the other into SolidCAM. I'm not complaining about Aspire because it does pretty good for it's intended purpose and it's a whole lot simpler to use than SolidCAM. Aspire is my go to CAM for quick and easy 2d stuff but SolidCAM is really nice for complex 3D models.
2686826869

[Chuck Keysor]

Here is a link to Vectric's training video on Rest Machining. The process seems a bit cumbersome, and one would think it could be/(Should be) automated, but it should point you in the right direction for doing multiple roughing passes. http://support.vectric.com/tutorials/V8/EfficientMachining3D/EfficientMachining3D_4.html Chuck

[BrandanS]

I'm not sure if it's possible to do what you want in Aspire, but other CAM systems do have this option. It's called REST machining (I think it stands for remaining stock). I own both Aspire and SolidCAM and I find that SolidCAM gives me a LOT more options for 3d machining. It has multiple options for creating work boundaries, and it also has several different machining stratagies instead of just offset or raster. I also find that SolidCAM results in a smoother surface finish because Aspire is pixel based which can result in jagged edges on steep surfaces. I've talked with Aspire about it and they gave me some tips on increasing the model resolution in the job setup menu but that still didn't completely help. Below are 2 screenshots of the exact same file that was created in Rhino but one was imported into Aspire and the other into SolidCAM. I'm not complaining about Aspire because it does pretty good for it's intended purpose and it's a whole lot simpler to use than SolidCAM. Aspire is my go to CAM for quick and easy 2d stuff but SolidCAM is really nice for complex 3D models.
2686826869

I also use SolidCAM, it's as easy as a click of a button and specifying what the previous tool diameter is.

@maverickx50 It does seems like you should be able to run with one less tool, however, I'm not machining it; you are. Are you using the roughing for wall or floor finishes? or both?

@pkirby [OFFTOPIC] I'm curious about how you ran into SolidCAM. Do you primarily use SolidWorks for your CAD? I've noticed a few bugs with SolidWorks 2016 itself, but also a bug withing SolidCAM, wherein my toolpaths, would suddenly ALL need to be recalculated if I was trying to modify feeds and speeds (which is weird). In fact, I couldn't even re-lay the geometry. After trying to redraw the exact same Sketch, and slowly losing all my previously calculated toolpaths, I became frustrated. I closed both SolidWorks and SolidCAM, reopened the file, and then suddenly everything started working again. Just a tip in case it happens to you.

[BrandanS]

Not that strange. A 10" X 10" square 3d shape maybe 5/8" deep may take 8 hours to cut with a 3/16" ball end-mill. By attacking it with first a 5/8" End mill then a 1/4" end mill and finishing up with a 3/16" I can reduce my total cutting time to less than 2 hours. Not counting the 2 extra tool changes of course. But I have extra collets & collet nuts etc so can have them and a next cut tool ready to go with little lost time. Now if I can take the air cutting out of the equation I'll save another 30 min or more.

The Z depth is not the answer as the smaller cutting tool comes with cut depth per pass limits built into the equation. I'd still be cutting a lot of air at the top of the 3D image is usually pretty close to the top of the material zero


Here is another Aspire rest machining tutorial, if it's of any help :D:

https://www.youtube.com/watch?v=itEhtQ3KVSY

[Burkhardt]

It can sometimes be much more time-efficient (and easier on the cutting edges) to machine a roughing pass all at once at full depth but with small path distance (more side-milling than end-milling). If the ballend flutes are long enough, I usually omit the roughing tool path altogether and make a first finish pass with a 1/4" or 1/2" ballend bit, maybe 20/1000 path distance, leaving a thin skin and then a final finish pass with the desired small radius ballend bit. However, you must start the raster outside the workpiece for this method and not have deep dips in the target surface where the bit will try to suddenly dive into. If you keep the tool path distance small enough you can go pretty deep, even with a 1/4" bit and let the upper section of the flutes do more work.

[pkirby]

I also use SolidCAM, it's as easy as a click of a button and specifying what the previous tool diameter is.

@maverickx50 It does seems like you should be able to run with one less tool, however, I'm not machining it; you are. Are you using the roughing for wall or floor finishes? or both?

@pkirby [OFFTOPIC] I'm curious about how you ran into SolidCAM. Do you primarily use SolidWorks for your CAD? I've noticed a few bugs with SolidWorks 2016 itself, but also a bug withing SolidCAM, wherein my toolpaths, would suddenly ALL need to be recalculated if I was trying to modify feeds and speeds (which is weird). In fact, I couldn't even re-lay the geometry. After trying to redraw the exact same Sketch, and slowly losing all my previously calculated toolpaths, I became frustrated. I closed both SolidWorks and SolidCAM, reopened the file, and then suddenly everything started working again. Just a tip in case it happens to you.
My background has always been with AutoCAD and I just got SolidWorks/SolidCAM this summer because there were some parts I needed to make that were not possible with Aspire. I've been banging my head against the wall trying to learn SolidWorks because it is nothing like AutoCAD! I haven't run into the bug you're talking about (although I have had others) but I appreciate the heads up.

[maverickx50]

My background has always been with AutoCAD and I just got SolidWorks/SolidCAM this summer because there were some parts I needed to make that were not possible with Aspire. I've been banging my head against the wall trying to learn SolidWorks because it is nothing like AutoCAD! I haven't run into the bug you're talking about (although I have had others) but I appreciate the heads up.

I worked with and even taught SolidWorks. After retirement I no longer had access to a SolidWorks key code # and at over $4000 + annual maintenance fee of over $1000 just can't justify that expense. Sure miss it tho.

[cowboy1296]

i do primarily 3-d. there maybe easier and faster ways to do it but i always do one roughing tool path followed by the finishing tool path. Now what i do is part time so if i were a shop owner and time is money i would always look for faster methods.

[Brady Watson]

1) Do your roughing with a large square end bit. Unless you are cutting aluminum or dense plastic, more than one roughing pass is not necessary. Every model is different. Listen to what your gut tells you.

2) Do as many finishing toolpaths as is required given the material density & resolution of the details on the model, using a coarse stepover - (E.G. - 20-40%) using a ball end mill.

3) Do your final 3D finishing pass with the smallest tool & tight stepover (8-12%) using a ball end mill.

BY carefully observing the toolpath previews you can gauge what is too much for a given diameter tool. In many cases it is possible to isolate spare areas using a vector to constrain the finer 'roughing pass' (really one of the finishing passes @ coarse SO) in order to save time by cutting down on air cutting.

Careful vector creation for the purposes of constraining the 3D toolpaths is critical and will pay dividends in time savings and overall quality.

There are many ways to do rest machining depending on what software you run. However, this is akin to automatic nesting of 2D parts. Your brain is more efficient than any algorithm.

-B