Final little finish passes

[Kyle F]

I am working on a fun little 5axis project. It has a handful of .06 radii corners on it, and I pre-drill where I can with a .12 dia drill. I then rough the part with 3/8 -- 1/4 -- 1/8 endmills and after most of my finish passes I am left with what is pictured here.

So I really just have a few cusps and tight corners that need finishing. so I have a necked back .118 dia 3flute endmill with .177 length of cut for this. My problem is that widdling these little sections and getting a decent finish isn't necessarily hard, it's just taking too long haha! At most there is probably .008 stock left in tiny sections. Right now I'm going about it running S6000 F10. and in some of the real tight sections going as low as s4000 f5. taking .175 depth cuts and 1 spring pass. It's got a teeny bit of chatter in sections but overall it's certainly acceptable. It's taking quite a while though and I've always read that tiny tools need a decent bite or else they vibrate but I've had pretty poor luck in the past when trying to finish small endmills with longer stickouts without slow SFM and multiple finish passes. the machine has 10k max spindle.

I'd love to hear how y'all would handle this little problem of mine! thanks for taking the time and reading this, appreciate any input

I work in a small job shop and my quantities typically usually max out at around 25 parts and most my jobs are new, but this one is actually a pretty high quantity (for me) and I'm running 4 parts on a tombstone so any cycle time I can cut off really helps!

 

[#Rekd™]

I would ramp down instead of taking a full depth cut.

[Kyle F]

25 minutes ago, #Rekd™ said:

I would ramp down instead of taking a full depth cut.

So essentially just draw some closed geometry in each corner and have the tool spiral down? I do love myself a helical ramp, I'm open to giving that a try! then once speeds/feeds are sorted out I can change angle of helix to speed it up and find a sweet spot.

[#Rekd™]

Not sure what toolpaths you are using.

If it is a 2D Contour there is a Ramp option and set it by depth. You don’t need a closed contour for this.

[JParis]

I deal with this and much smaller, on a daily basis....I ramp cut those corners and walls....

I do not "generally" drill those corners, our QC likes to bitch about finish. If I do, I will drill out by about .005" in the X & Y off the center and let the endmill finish it.

When I do get the occasional question on run times, I point out ALL of the small corners and small 3d blending a part requires...."small tools = time"

I minimize the cutting by drawing lines in the corner, along with a reference dia of the last tool size that cut in there and I'll extend the wall lines out far enough to cover the small cusp + a small fudge factor...in doing so it allows me to minimize the amount of cutting the small tool must do, helping keep its time cutting to a minimum.

[cruzila]

I do this quite often. Drilling corners is a concept of the past. The re-machining feature in contour is pretty effective without having to recreate any geometry. play with the numbers to get your results. The option I use most often is roughing tool dia. Keep tool down and in lead in/out use a big radius angle to get the tool back around.

Currently I am doing a stainless part with a 125r through about 3-1/2 thickness. 

[Kyle F]

On 10/13/2023 at 9:28 PM, #Rekd™ said:

Not sure what toolpaths you are using.

If it is a 2D Contour there is a Ramp option and set it by depth. You don’t need a closed contour for this.

oh that's wild for some reason I thought it had to be a closed contour. whoops! thank you.

On 10/14/2023 at 6:31 AM, JParis said:

I deal with this and much smaller, on a daily basis....I ramp cut those corners and walls....

I do not "generally" drill those corners, our QC likes to bitch about finish. If I do, I will drill out by about .005" in the X & Y off the center and let the endmill finish it.

When I do get the occasional question on run times, I point out ALL of the small corners and small 3d blending a part requires...."small tools = time"

I minimize the cutting by drawing lines in the corner, along with a reference dia of the last tool size that cut in there and I'll extend the wall lines out far enough to cover the small cusp + a small fudge factor...in doing so it allows me to minimize the amount of cutting the small tool must do, helping keep its time cutting to a minimum.

I'll definitely try the ramp. and generally if I ever use drills to help rough I also will keep them a few thou off of the walls. This is an odd situation where the added cycle time wasn't worth the slightly improved finish in the corners due to the quantity of the job and the tolerance on the finish. 

On 10/14/2023 at 9:13 AM, cruzila said:

I do this quite often. Drilling corners is a concept of the past. The re-machining feature in contour is pretty effective without having to recreate any geometry. play with the numbers to get your results. The option I use most often is roughing tool dia. Keep tool down and in lead in/out use a big radius angle to get the tool back around.

Currently I am doing a stainless part with a 125r through about 3-1/2 thickness. 

that is another old bad habit of mine I need to get rid of! I never use re-machining option on the contour setting and this is a great time to put it to use. I have a handful of different 2d contours set to single radii each with varying lead-ins/lead-outs and it's a whole lot of added toolpaths for nothing lol. I appreciate the input. Excited to put this to use in my program today and demo out tomorrow!

[JB7280]

On 10/13/2023 at 10:28 PM, #Rekd™ said:

Not sure what toolpaths you are using.

If it is a 2D Contour there is a Ramp option and set it by depth. You don’t need a closed contour for this.

I tried this after reading your comment, as I'm in this same situation quite a bit.  When I use ramp on an open contour, it wants to climb AND conventional mill. Is there a way to avoid that? 

 

Maybe I'm misunderstanding the method.  

 

[JParis]

On 10/14/2023 at 10:13 AM, cruzila said:

The re-machining feature in contour is pretty effective without having to recreate any geometry

Here's why I don't use that often..

By creating a closed contour, I can set a reasonably steep ramp around the contour. In the end, many times that is faster that the re-machining option.

I can take 2 ramped passes around when using the remachining option I generally need many more step downs.

[JB7280]

4 minutes ago, JParis said:

Here's why I don't use that often..

By creating a closed contour, I can set a reasonably steep ramp around the contour. In the end, many times that is faster that the re-machining option.

I can take 2 ramped passes around when using the remachining option I generally need many more step downs.

So you basically create a circle, instead of just using the radius, and ramp/spiral down at like, 15-20deg?

[JParis]

4 minutes ago, JB7280 said:

So you basically create a circle, instead of just using the radius, and ramp/spiral down at like, 15-20deg?

No...a round cornered triangle

 

[Leon82]

1 hour ago, JParis said:

Here's why I don't use that often..

By creating a closed contour, I can set a reasonably steep ramp around the contour. In the end, many times that is faster that the re-machining option.

I can take 2 ramped passes around when using the remachining option I generally need many more step downs.

plus re machining doesn't respect internal radius

[crazy^millman]

2 minutes ago, Leon82 said:

plus re machining doesn't respect internal radius

Dynamic Contour does. I will draw a radius bigger than the previous tool. I am going into a .03R corner and my last tool was .5 endmill I then draw a .3 radius into that corner. I then trim the wireframe around the .03R to then use a .06 endmill to take within .001. Then when I take my finish pass all the away around the feature I get a nice looking part with stock where i expected it. I still will drill over 10XD and 20XD corners on 3 Axis work leaving .002 to .005 to finish with the endmill. On 5 axis part then I explore different methods like Barrel Tools or other option if the part and shape allow it.

[JB7280]

2 hours ago, JParis said:

No...a round cornered triangle

 

oh ok, that makes sense.  

[#Rekd™]

3 hours ago, JB7280 said:

I tried this after reading your comment, as I'm in this same situation quite a bit.  When I use ramp on an open contour, it wants to climb AND conventional mill. Is there a way to avoid that? 

 

Maybe I'm misunderstanding the method

Then you need to create a small triangle like JP stated. 

[JB7280]

1 hour ago, #Rekd™ said:

Then you need to create a small triangle like JP stated. 

I hadn't seen that yet when I had posted. I have a part I'm working on now with lots of pockets with small radii so I'll be giving it a shot.  

[#Rekd™]

On 10/13/2023 at 7:52 PM, Kyle F said:

I'm open to giving that a try! then once speeds/feeds are sorted out I can change angle of helix to speed it up and find a sweet spot.

If you have the funding buy yourself HSM Advisor (Speeds and Feeds app). The have a free version call FSWizard but the HSM Advisor offers more information and gives you access to FSWizard Pro.

I bought personally it a while back on a recommendation from @crazy^millman best $195.00 (life time license) I ever spent for drilling small holes among other features it has. 
 

We use a lot of Harvey tools for small end mills under 1/8” and Helical Solutions for 1/8” and larger. They have an excellent Machining Advisor application on their website but it is only for their products.

[crazy^millman]

I have used HSMWorks since it first came out. I have recommned it to 100's of customers and they all like it also.

Same with Varco Reports many of our customers purchased after see the quality of what we were giving them using it. Jim and talk from time to time and glad to know him.

X+ is a great setup tool also and seen some amazing things Robert (Zoober) did with it that was world class.