I have a toolpath I cut out with a .25" end mill. However the diameter prevents me from getting into some tight areas. The clear solution to me is to generate a second toolpath using a .125" end mill, but I don’t want it to run the entire profile again with the .125" - just clean up the areas the .25" couldn’t fit into.
Is there any way to do this? Or do I basically have to copy the vectors and crop out everything but the areas I want it to hit?
I am assuming you are cutting a pocket…
When you create your toolpath, choose the small bit for the toolpath (0.125") then select the larger bit in the area just below Tool called “Use Large Area Clearance Tool” and select your larger bit (0.25")
The pocket tool path allows a clearance tool and a smaller tool for detail
Hmmm no in this case it’s a profile… imagine cutting out a name in cursive, there are corner areas that you need a smaller end mill to get into.
If I use a pocket function to cut out the letters, it would take longer than just running the 1/8 toolpath
Sorry, you will need to just use the smaller bit.
Maybe this image helps… this is with a .25" toolpath already run, and now the blue lines are the .125" path… you can see it only really needs to clear out a bit of material in a few places:
Personally, I would just use the smaller bit for the profile cut.
it’s only .75 MDF, but I figure i can really push it fast with a larger end mill… I’m doing about 14 of these in a run so a tool change isn’t a big deal
Here’s the problem I’m trying to solve:
If you run the 0.25" bit first, you can run the 1/8" bit faster as it only has a little to clear, but if you go too fast, it will hit spots that are not touched and you risk breaking the bit.
You could use the offset tool to draw another vector .25 inch outside the edge profile you are using now. Then perform a pocket toolpath between the new vector and your existing edge. Then you could use the .25 bit for clearance and the .125 for cleanup.
Clever, I like it… I’ll give that a try 
thanks
You may need to make the new vector offset slightly larger than .25 to be sure it can fit the .25 bit. Two toolpaths will be created from the pocket, and you can see in the simulation what is removed with each one.
Also tabs needs to be worked out differently… hmmmmm
Okay I have another idea to try… I might just break up the lines into segments rather than closed paths and have it run along those… I’ve done something similar int he past and it seems to work on segments
The profile tool path will work on segments
yeah just tried that… it did reduce time but suddenly the tool couldn’t fit in areas it can when I don’t break it into segments. Weird.
I might just bite the bullet on it and eat the extra 2.5 hours per run 
so one thing that you might try is the drilling tool path in aspire to clean up the tight corners all your are trying to do with the .125" tool is put in a .0625" radius instead of the .125" radius created with the .25"
so in every tight corner draw a circle and then use the drilling tool path to drill straight down in that area and if you get your holes offset correctly it will look like you used a .125" tool on the whole thing
if you shoot me a crv file I can show you what I am talking about but its going to be super fast compared to trying to do another profile pass
Mdf is actually really hard on tools that’s why only carbide or diamond tools should be used
Plus the Op is cutting .75" thick Mdf and general rule of thumb is never go x4 over diameter of tool and in the case of the .125 inch tool that’s .5"
Really you would have to take lots of super shallow passes with a .125 tool versus
I say hog out the most material you can and then if you must reduce the inside corner radius by .0625 the go back and drill the corners with the smaller tool
The .25" tool will make a .125" inside radius and the .125" tool will make a .0625" radius so by going back with the .125" tool after the .25" tool you only gain a .0625 tighter radius so I am not sure if it’s worth it but if the design calls for it then you must do what you gotta do and I think a drilling Tool path would be the fastest way to accomplish that
