Problems with Surface High Speed Toolpaths- Hybrid

[masterslam]

I like this tool path, but can not get it to give me a good part a lot of times. I am machining a Broach tool out of 5/8" round stock, it has several standing cutting edges. I am using the Hybrid toolpath to finish it with a .093 ball endmill, . at several points in the toolpath the cutter transitions to another location by staying right on the surface and going up and over to the other side of the part, when doing this it will blow right thru a shart edge by several thousands and leave a gouge or cut a sharp corner right off. any sugestions, i have tried adjusting everything, somethimes it will change the path but will just do the same thing in another spot. Again, i like the way this toolpath cuts but its screwed me over every time i try to use it.

[masterslam]

anybody have any ideas?

 

 

[peon]

That may happen when using "Minimum Distance" in your linking parameters. Switch to "Minimum Vertical Retract" or "Full Vertical Retract".

[Chris Rizzo]

at several points in the toolpath the cutter transitions to another location by staying right on the surface and going up and over to the other side of the part,

 

I have run into this as well. When moving from one pocket to another, it basically runs across the top of the part. Clear as day in verify. I'd send it into qc.

[Thee Rickster ™]

Happens to me with pencil as well when using virticle retract.

If you have 'keep tool down' selected

And a large number in there ( to reduce retracts)

it rides the distance over to the next area and

Leaves a trail, so to speak , which in my eyes is a gouge.

When using min distance make sure you have .100" in the

Clear

 

So I use min distance ... But don't use keep tool down.

Same when using hybrid and have not had it happen since.

 

Definately send it in, and ask then to try it in x6

Because there are no more fixes for x5.

[Ocean Lacky™]

On the Cut Parameters page, what are your settings for Keep Tool Down?

I try to remember to set mine to 100% of tool diameter as sometimes Mastercam will randomly set it at 1327% which will yield the same results as you are getting.

[Thee Rickster ™]

mine randomly sets to 0.053.

 

The number you put in has t be slightly smaller then the smallest jump from

pocket to pocket , or core to core, otherwise it trails over those areas.

 

The larger the number the more trails depending on the distances between jumps.

 

Thats how it does it here but regardless it SHOULD not be violating the surfaces....period