JB7280

Need some advice milling deep slot

Recommended Posts

Not Mastercam related, but you guys are pretty smart, so I'm gonna ask here.  I have a 6061 part with 2 slots, about 11mm wide and 5" deep.  The slot ends up through.  I am able to attack them from both sides, however there are other features next to them that require a minimum of 3.25" extension.  I'm using a 3/8" endmill with a reduced neck and 1/2" for length.  Not exactly the greatest set of requirements, but that's life.

 

I've tried all sorts of different things. 

Helicals MAP suggestions, HSM Advisor's suggestions, and everything in between.  1500-15000 rpm.  I've held it in a lyndex SK10, and a VC13 holder. As of now I've got nothing but chatter, broken tools, and broken dreams.  If anyone has any suggestions, I'd really appreciate it!!!

  • Sad 1

Share this post


Link to post
Share on other sites

For starters, I would use several endmills to get there...each being longer than the next...ultimately the longest endmill would only be nibbling at the depths but it would be limited in cuts to only what it can reach..

I would use a drill to remove as much material as I could, using something like a 65-70% stepover...

Finish by using ramp cuts to keep the tool engaged..speeds & feeds will be varied by the different reach tools...lonest crawling along

  • Like 5

Share this post


Link to post
Share on other sites
17 minutes ago, JParis said:

For starters, I would use several endmills to get there...each being longer than the next...ultimately the longest endmill would only be nibbling at the depths but it would be limited in cuts to only what it can reach..

I would use a drill to remove as much material as I could, using something like a 65-70% stepover...

Finish by using ramp cuts to keep the tool engaged..speeds & feeds will be varied by the different reach tools...lonest crawling along

What do you mean by drilling with 70% stepover?  Are you referring to a flat bottom drill?

 

I will check the option of using multiple tools tomorrow.  Unfortunately because of those raised features next to the slot, even the shortest tool will be at least 5xD, which is still better than the 10d I'm currently working with.

Share this post


Link to post
Share on other sites

Do you have a wire EDM? 

I have done this in the past with a ramping contour toolpath.  With a shallow pitch and full width of cut, the tool will be somewhat stabilized by cutting beyond center as you ramp down.  A corner radius will help also, anything that puts the majority of the cutting force straight up the centerline of the tool will help.

The biggest problem is getting chips out...

Share this post


Link to post
Share on other sites
3 minutes ago, bd41612 said:

Do you have a wire EDM? 

I have done this in the past with a ramping contour toolpath.  With a shallow pitch and full width of cut, the tool will be somewhat stabilized by cutting beyond center as you ramp down.  A corner radius will help also, anything that puts the majority of the cutting force straight up the centerline of the tool will help.

We do, but this part is bigger than our Edm.  Truly would have been the best option.  When you say shallow ramp, how shallow would you suggest? I tried as low as 3*.  It seemed to be cutting nicely at a heavier ramp and, but the ramp was being the flute length.   What speeds and feeds would you suggest?

Share this post


Link to post
Share on other sites
2 minutes ago, JB7280 said:

We do, but this part is bigger than our Edm.  Truly would have been the best option.  When you say shallow ramp, how shallow would you suggest?  What speeds and feeds would you suggest?

Maybe .025 - .030 depth per pass.  [email protected] Maybe.  Hard to say without seeing it firsthand.

  • Like 2

Share this post


Link to post
Share on other sites
4 hours ago, bd41612 said:

Maybe .025 - .030 depth per pass.  [email protected] Maybe.  Hard to say without seeing it firsthand.

Thanks.  The slots are already cut through on this part, but I plan to get a block of material and try this, as well as Predrilling and using constant Z depths.

Share this post


Link to post
Share on other sites

I would drill the ends of the slot through first, both for relief of the corners, and to allow chips to exit. If you have coolant through, this would help flush chips.

https://www.helicaltool.com/products/tool-details-83736

Here is a 3/8" diameter, high-feed endmill, which would do a nice job in most materials. It is meant for steels and cast iron, but I've made them work in Aluminum in a pinch.

I'd stick with .03-.04 inches per depth pass, using Contour Ramp > Plunge. I would typically run center-passes, with a plunge at the end of each pass, then come back the other way. Finally, I'd use a Ramp Contour to finish. Probably a 0.004-0.01 finish pitch. You don't really have a full corner radius, so you compensate with a tighter z-pitch for the ramp.

  • Like 1

Share this post


Link to post
Share on other sites

I once had to make a few grooves 1.6 mm wide and 20 mm deep. I created a surface in the middle of the groove and created a toolpath where the tool is going like a sewing machine some 2000 mm up and down and a increment horizontal move of 0.05 mm. I could have EDMed it , but the manual polishing after the burn 

made me mill . the grooves were altogether 1.5 meters long in 0.5 meter chunks. The material was of course steel ,HRC 33. I think only 3 or 4 end mills were used.

Gracjan . 

Share this post


Link to post
Share on other sites

 

8 hours ago, Colin Gilchrist said:

I would drill the ends of the slot through first, both for relief of the corners, and to allow chips to exit. If you have coolant through, this would help flush chips.

https://www.helicaltool.com/products/tool-details-83736

Here is a 3/8" diameter, high-feed endmill, which would do a nice job in most materials. It is meant for steels and cast iron, but I've made them work in Aluminum in a pinch.

I'd stick with .03-.04 inches per depth pass, using Contour Ramp > Plunge. I would typically run center-passes, with a plunge at the end of each pass, then come back the other way. Finally, I'd use a Ramp Contour to finish. Probably a 0.004-0.01 finish pitch. You don't really have a full corner radius, so you compensate with a tighter z-pitch for the ramp.

Here's a screenshot of the slot.  I was wrong about the slot, it's actually .657 wide and I'm roughing it with .025 left per side.  The corners of the slot are 5mm rad, so I wouldn't be able to drill 4 holes at the corners unless I went down to like 1/4" drill. 

  • Would you recommend I do that, Or just drill one hole as big as i can? 
  • If I were to use that high feed mill, would I do better to have full material there, or holes drilled along the slot to remove the material?  
  • What kind of parameters would you try, to use that feedmill in aluminum?

I had no idea thats what Ramp > Plunge did!!!  I always thought it was for plunge milling, and I never messed with it.  Whats the difference though, between that, and just a contour with depth cuts?  Aside from plunge not using entry/exit, I couldn't notice a difference.

 

EDIT - I think I figured out the difference.  The ramp plunge will feed on it's Z moves and not retract. Any other difference?

 

fyi, those little radii on the ends don't go all the way down.  They're not an issue.

slot.jpg.72ebd064072fac0a4dedac5ad88064dd.jpg

Share this post


Link to post
Share on other sites

Without your exact part, it's always difficult of course, but I thought I'd throw this out there if you have access to Multiaxis toolpaths.    A lot of people don't know that you can convert a most of the advanced multiaxis toolpaths (Unified, Morph, Parallel, etc) to a plunge rough.

I agree with JParis that I'd try plunge roughing this material out.  You should be able to get a 10.25mm or so drill, and that should be accurate enough to only leave like .375mm of material on the walls, which will make your job a lot easier.  One note is that you can't "use a drill" for this toolpath, so I just defined an endmill with the same parameters as my drill.

The first toolpath is just how to set up a Parallel to cut the wall, the Cut Pattern page is set up to follow the long wall with a single pass:

image.thumb.png.92bf7af6aa0188bf5085bc43523f2e74.png

The offset is controlling how far away from the wall to stay ((11mm slot-10.25 drill)/2 = .375mm).

Tool Axis Control is set to 3 Axis.

I'm using the collision control to trim away from the edges:

image.thumb.png.3dba2b32fd4337edb361103563b278e8.png

I then Copied the toolpath and converted it to a plunge roughing just so you could see the difference:

image.thumb.png.19e095503b49d004e509440c2ee027ee.png

image.png.4302a441a04b68a44800e69f49b49bf6.png

 

I'd just finish with a reduced neck endmill doing a spiral (contour ramp).    There'd only be .375mm (.014") of material, so two passes should do it with a 10.5mm endmill, possibly 3 depending on harmonics..

Parallel Plunge.zip

  • Like 1

Share this post


Link to post
Share on other sites
5 minutes ago, Aaron Eberhard - CNC Software said:

Without your exact part, it's always difficult of course, but I thought I'd throw this out there if you have access to Multiaxis toolpaths.    A lot of people don't know that you can convert a most of the advanced multiaxis toolpaths (Unified, Morph, Parallel, etc) to a plunge rough.

I agree with JParis that I'd try plunge roughing this material out.  You should be able to get a 10.25mm or so drill, and that should be accurate enough to only leave like .375mm of material on the walls, which will make your job a lot easier.  One note is that you can't "use a drill" for this toolpath, so I just defined an endmill with the same parameters as my drill.

 

Thank you for that!  When you say to drill it, I'm guessing you're referring to a flat bottom drill??

Share this post


Link to post
Share on other sites
5 minutes ago, JB7280 said:

Thank you for that!  When you say to drill it, I'm guessing you're referring to a flat bottom drill??

Yeah, I'd want an inserted gun drill probably, if money were no object.. But since it's just 6061, a solid carbide with through tool coolant should be fine.   If you're REALLY stuck without through tool, solid carbide with pecks, but that'll be REALLLLLLY tedious.

Ooh, I just had another thought.. what's the call out for surface finish on the slot?  You'd probably be able to finish machine the wall a lot easier with a barrel mill using Waterline.   There'd be tons less chatter that way than trying to use a reduce neck endmill... But you'll have scallops at some level.  I don't know if they make any long enough, though.

  • Like 1

Share this post


Link to post
Share on other sites
9 minutes ago, JB7280 said:

Thank you for that!  When you say to drill it, I'm guessing you're referring to a flat bottom drill??

I can't think of any reason you would want to pre-drill 6061, just send in the endmills and call it a day, some good cutting strategies above.

  • Like 2

Share this post


Link to post
Share on other sites
1 minute ago, [email protected] said:

I can't think of any reason you would want to pre-drill 6061, just send in the endmills and call it a day, some good cutting strategies above.

The dia to length ratio,,,is why...

At shallow depths, I would agree, not a big reason to do so....but as it's a long reach on a smallish size tool...removing as much excess material ahead of time can only help..

  • Like 2

Share this post


Link to post
Share on other sites

It could happen also, the drill may wander,

I always suggest to only pre-drill on hard materials like stainless steel, and only in specific situations, here its unnecessary as a 3/8 endmill is unlikely to snap, if programmer properly!

i mean i guess it depends on the quality of the tools you have available

Share this post


Link to post
Share on other sites
11 minutes ago, [email protected] said:

i mean i guess it depends on the quality of the tools you have available

In my case, nope...just years of experience

Share this post


Link to post
Share on other sites
29 minutes ago, Aaron Eberhard - CNC Software said:

Yeah, I'd want an inserted gun drill probably, if money were no object.. But since it's just 6061, a solid carbide with through tool coolant should be fine.   If you're REALLY stuck without through tool, solid carbide with pecks, but that'll be REALLLLLLY tedious.

Ooh, I just had another thought.. what's the call out for surface finish on the slot?  You'd probably be able to finish machine the wall a lot easier with a barrel mill using Waterline.   There'd be tons less chatter that way than trying to use a reduce neck endmill... But you'll have scallops at some level.  I don't know if they make any long enough, though.

Nothing crazy, it's just a pass-through for wires.  Falls under the general profile tolerance.  The end size is actually 16.7mm so I think I'll look for a 14.5mm or 15mm drill?  Then just clean the cusps, and come back and finish the rest after stress relief.  I think some scallops wouldnt be an issue.  I did some looking on Emuge, and Mitsubishi's offerings, and wasn't able to find anything that would be long enough in a barrel mill.  I like the idea though.

  • Like 1

Share this post


Link to post
Share on other sites
46 minutes ago, JParis said:

In my case, nope...just years of experience

I don't have much experience, but i figure, if it works in the simulator...

Share this post


Link to post
Share on other sites
4 minutes ago, [email protected] said:

I don't have much experience, but i figure, if it works in the simulator...

lol, no you don't   you've likely done something similar in the real world..   :)

and if you're doing a low qty...you'll likely get through it...

I come at things from a long term, we're making 5,000 plus of these "thingamajigs"  ....I need a process that will be repeatable, not overly eat up tools and standup over the long haul...that's how I approach many things at this point...

Just a different approach from a longer view purpose  :)

  • Like 3

Share this post


Link to post
Share on other sites
On 9/21/2021 at 8:41 AM, Aaron Eberhard said:

Without your exact part, it's always difficult of course, but I thought I'd throw this out there if you have access to Multiaxis toolpaths.    A lot of people don't know that you can convert a most of the advanced multiaxis toolpaths (Unified, Morph, Parallel, etc) to a plunge rough.

I agree with JParis that I'd try plunge roughing this material out.  You should be able to get a 10.25mm or so drill, and that should be accurate enough to only leave like .375mm of material on the walls, which will make your job a lot easier.  One note is that you can't "use a drill" for this toolpath, so I just defined an endmill with the same parameters as my drill.

The first toolpath is just how to set up a Parallel to cut the wall, the Cut Pattern page is set up to follow the long wall with a single pass:

image.thumb.png.92bf7af6aa0188bf5085bc43523f2e74.png

The offset is controlling how far away from the wall to stay ((11mm slot-10.25 drill)/2 = .375mm).

Tool Axis Control is set to 3 Axis.

I'm using the collision control to trim away from the edges:

image.thumb.png.3dba2b32fd4337edb361103563b278e8.png

I then Copied the toolpath and converted it to a plunge roughing just so you could see the difference:

image.thumb.png.19e095503b49d004e509440c2ee027ee.png

image.png.4302a441a04b68a44800e69f49b49bf6.png

 

I'd just finish with a reduced neck endmill doing a spiral (contour ramp).    There'd only be .375mm (.014") of material, so two passes should do it with a 10.5mm endmill, possibly 3 depending on harmonics..

Parallel Plunge.zip

I'm trying this but cannot get it to function.

 

 

Share this post


Link to post
Share on other sites

Just a little update on this in case anyone else is in a similar situation.  

 

I ended up running a .492" drill through the slot.  5 holes, spaced evenly (the drill was already in the machine for another part)  After that I created a dynamic toolpath using the pre-drilled holes as air regions, although I made the actual air regions .472" diameter, to avoid any small slivers on such a long ratio tool.  

 

500SFM/.004ipt, 10% stepover, .450"doc and it sounds great.

 

Thanks for your suggestions

  • Like 3

Share this post


Link to post
Share on other sites
On 10/13/2021 at 9:30 AM, jean said:

I'm trying this but cannot get it to function.

 

 

Sorry, I missed this.. Can you post the file/toolpath that you can't get working?

3 hours ago, JB7280 said:

Just a little update on this in case anyone else is in a similar situation.  

 

I ended up running a .492" drill through the slot.  5 holes, spaced evenly (the drill was already in the machine for another part)  After that I created a dynamic toolpath using the pre-drilled holes as air regions, although I made the actual air regions .472" diameter, to avoid any small slivers on such a long ratio tool.  

  

500SFM/.004ipt, 10% stepover, .450"doc and it sounds great. 

 

Thanks for your suggestions

That's awesome to hear you got it. Thanks for following up!

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us