3d surfacing stepover question

[MILLRUNNER]

Doing more surfacing stuff. Let's say I'm using a 1/8" ball to rough. I was wondering what stepover would be about the max I can leave that a finish pass won't choke on.

 

Initially I was going to use a 1/16" ball to finish, but if I can do it with that same (size) 1/8", I feel like i can push it faster and it would eliminate a tool change.

 

Assuming I do just use one size of tool (1/8"), the way I have it programmed now is to do a .006" stepover and leave .003 on the drive surface for the rough pass. The finish pass is programmed with the same .006" stepover, but no zero material left on the drive surface.

 

Should I open up the stepover on the rough pass?

[jeff]

 

 

Should I open up the stepover on the rough pass?

I would at least double it. 

Unless you have a special circumstance where a larger stepover would hurt you.

[AMCNitro]

Depending on the material, you cold easily go .015 on the rough.  Also, whats your DOC on the rough?

[duckdogers]

I would double the rough stepover and depending on finish I always use a .002 or .003

[MILLRUNNER]

It is just a test, but the way the cut works is it initially starts off taking 0(zero) in the Z. It then progressively works down to a final depth of about .067".

 

That would mean that the most axial engagement the tool will see is .067", but the radial will never exceed the max stepover - currently .006"

 

I am cutting aluminum at the moment for the test, and the way I have my speeds figured are at S8350 / F4.2 on the rough pass, and S10K F12. on the finish.

 

10K is all I have at spindle.

 

If I double the rough stepover, that makes the axial cut .012", and the speeds I'm getting for that are S8350 / F3.3

 

--Changing from .006" to .012" brought my machining time down from 3hr 31min to 2hr 28min.

[tim_h]

Those Feed Rates seem REALLY slow.

[duckdogers]

Those Feed Rates seem REALLY slow.

I agree you can probably increase speeds and feeds ,its only aluminium

[AMCNitro]

Yeah, kinda of slow for the feed

[MILLRUNNER]

I'm running at 70% on speeds and feeds. Maybe should kick it up to 100%.

 

changing to 100% knocked of another hour or so.

 

Down to 1hr 33min.

[MILLRUNNER]

The new feeds at 100% are S10K F5.7 for roughing - max axial .067", stepover (radial) .012"

 

S10k F17 for finishing. max axial .003", Stepover .006"

[AMCNitro]

Can you shows what you are machining?

[crazy^millman]

The new feeds at 100% are S10K F5.7 for roughing - max axial .067", stepover (radial) .012"

 

S10k F17 for finishing. max axial .003", Stepover .006"

Why are you running that so slow? If I were using a 3 flute end mill for roughing I would be at 180 imp for roughing and 90 imp for finishing. If you are using a 2 flute you are at .001 per tooth reed rate which is rubbing off the material not cutting it off. Your surface finish should be dull. Kick it up and watch the finish get better and the job get done faster. You need to learn about speeds and feeds.

[Redfire427]

I hope those feedrates are at feet/meters per minute.

 

Carmen

[MILLRUNNER]

I don't know much about 3d surfacing, or optimizing feeds at the moment. I'm still trying to learn. Please excuse my ignorance.

 

I have used two online speed calculators, and trying to decide how to go further on them. I use FSwizard for the most part because it is free, but I have downloaded the trial of Gwizard. Gwizard seems to give a lot faster feed.

 

I just redid my toolpaths by double checking all my inputs. I am not exactly sure why I was getting such a low number, but I suspect it could have been the input of length. I thought that meant the length of the whole entire tool, not just the stickout from the holder. That changes things considerably.

 

Now I am getting this at 100% on FSWizard:

 

S10K F27.5 for roughing - max axial .067", stepover (radial) .012"
 
S10k F30.38 for finishing. max axial .003", Stepover .006"

[JoshC]

sounds like the calculators are not incorperating Radial chip thinning into the equations and perhaps giving you feedrates for a much larger width of cut.

[MILLRUNNER]

Can you elaborate on what exactly radial chip thinning is?

[JoshC]

There are a ton of sources online which go in detail on radial chip thinning and would do a much better job than i can explain. Here is a link to Mastercams website where they discuss RCT to get you started in the right direction.

 

http://www.mastercam.com/en-us/Communities/Blog/PostId/73/Mastercam-Radial-Chip-Thinning-Revisited

​

I think that link above goes over it very well, High feed milling cutters utilize the similar concepts but its axial chip thinning, Sandvic has a very good tip film which explains:

very well

[Redfire427]

I suspect that you are inputting the feed based on each revolution, rather than "per tooth per revolution ". 

 

Example: If you calculator shows .005" and you are running at 10K rpm, that translates to 50 inches per minute feedrate, however, the .005" should be per tooth. So if you have a 4 flute endmill, that translates to .020" per revolution, or, 200 inches per minute feedrate. 

 

Radial chip thinning is a whole other subject. You might be best to do a Google search on that to see a graphic and wrap your head around that. Basically it allows you to increase your feedrate significantly when cutting a small amount of material at the side of the tool.

 

Carmen

[crazy^millman]

I don't know much about 3d surfacing, or optimizing feeds at the moment. I'm still trying to learn. Please excuse my ignorance.

 

I have used two online speed calculators, and trying to decide how to go further on them. I use FSwizard for the most part because it is free, but I have downloaded the trial of Gwizard. Gwizard seems to give a lot faster feed.

 

I just redid my toolpaths by double checking all my inputs. I am not exactly sure why I was getting such a low number, but I suspect it could have been the input of length. I thought that meant the length of the whole entire tool, not just the stickout from the holder. That changes things considerably.

 

Now I am getting this at 100% on FSWizard:

 

S10K F27.5 for roughing - max axial .067", stepover (radial) .012"

 

S10k F30.38 for finishing. max axial .003", Stepover .006"

 

I was not trying to be mean, but even those seems extremely slow to me for aluminum, All out is how I have always run aluminum. I would kick a Bridgeport up to max rpm and kick the feed on the table up to as fast as it would go cutting aluminum. I train customers all the time on on things like this and get the book and follow what the book recommends for the speeds and feed for the tool on that material to get started then you need to go out and see what the tools the machine tell you about the cut.