Do you guys drill out corners where applicable

[lowcountrycamo]

In the past I have drill corners on deep pockets  but have gotten away from that.  Not sure why.

does anyone here practice that?   I have also heard of plunging corners as well. 
thanks,

steve austin

[AMCNitro]

Youre adding run time, the endmill will go there anyways.

[JParis]

Only in an a rare circumstance. Something that used to be common place that few perform any longer.

[cncappsjames]

Rarely.

Like never in the last 15 years.

[Aaron Eberhard]

In general practice, only if I'm doing a clearance pocket (i.e., I actually want circles in the corner so you can remove a plug), and it's <= the endmill diameter.

I did have a small aluminum aerospace bracket with pockets I helped with a few years ago that had really thin walls (think RF components, each in their own little "pocket" to keep them isolated).  I ended up drilling out the corners before any roughing was done because you could see a bit of distortion  bowing out the corners of whatever pocket was done second.  Switching to a smaller endmill would have taken care of it, but I ran the numbers on their machine and it was faster to drill out the corners to reduce that load than it was to switch to the smaller mill.  There were a lot of pockets   I believe it was really an issue of the thru coolant and/or chips pushing on the walls a bit during evac?

[Matthew Hajicek - Singularity]

I have some families of parts with pockets with 180 degree clearance corners, and I'll pre-drill those.  Otherwise the cutter would be in a full slotting condition as it enters the corner.  The alternative would be to go to a smaller cutter, but that would negatively impact cycle time.

 

This kind of clearance corner, but deeper:

[JB7280]

Hopefully this doesn't hijack the topic, but I feel like it's on the same subject.  Do any of you guy use the corner slowdown function in the arc filter section?  I do a lot of deep(ish) pockets.  Nothing crazy, but 6-8xD, and always seems to require a couple spring passes to nail the corner rads.  

[JParis]

4 minutes ago, JB7280 said:

Do any of you guy use the corner slowdown function in the arc filter section?  I do a lot of deep(ish) pockets.  Nothing crazy, but 6-8xD, and always seems to require a couple spring passes to nail the corner rads.  

I do a ton of this kind of stuff AND deeper....no..the Mazaks we can use Contour Control and we do, A LOT!

[JB7280]

21 minutes ago, JParis said:

I do a ton of this kind of stuff AND deeper....no..the Mazaks we can use Contour Control and we do, A LOT!

I'm not familiar with Mazak Contour control.  Is that similar to IPC on a Matsuura?

[cruzila]

With the wireframe radius clearance option there is little need for that much corner if you are designing some sort of tooling. If it is a part, obviously not negotiable.

 

I agree with all of the comments. No real need for a drill. The only exception I could think of is if the finish tool is really close to the size and you want to reduce tool deflection.

[Matthew Hajicek - Singularity]

Well, I guess I learned something.  I tried the same program, skipping the corner drills, and it worked just fine.  Tool life is still acceptable.

[cncappsjames]

In "engineer's" favorite corner radii... 1/8 and 1/4... metric tools are your friend. 6mm and 12mm respectively.

[Colin Gilchrist]

On 12/8/2022 at 1:27 PM, JB7280 said:

Hopefully this doesn't hijack the topic, but I feel like it's on the same subject.  Do any of you guy use the corner slowdown function in the arc filter section?  I do a lot of deep(ish) pockets.  Nothing crazy, but 6-8xD, and always seems to require a couple spring passes to nail the corner rads.  

To do this with finishing, I use "Change at Point" function, break the chain geometry before the corner, and use Change at Point to change the Feedrates on the chain itself. With 'Change at Point', this allows you to save those manual changes into the toolpath geometry, and then be able to make changes to the path, and still have the ability to regenerate your changes. (Still have to make the corner feed adjustments "manually" with Change at Point, if you want to change those sections.) This is a pain in some respects due to the manual intervention aspect, but allows you some serious control over the path results itself.

[Corey Hampshire]

41 minutes ago, Colin Gilchrist said:

To do this with finishing, I use "Change at Point" function, break the chain geometry before the corner, and use Change at Point to change the Feedrates on the chain itself. With 'Change at Point', this allows you to save those manual changes into the toolpath geometry, and then be able to make changes to the path, and still have the ability to regenerate your changes. (Still have to make the corner feed adjustments "manually" with Change at Point, if you want to change those sections.) This is a pain in some respects due to the manual intervention aspect, but allows you some serious control over the path results itself.

Pardon my ignorance, but where is "Change at Point" located? I see where this could be very powerful and wanted to play around with it, but can't seem to find it.

[Colin Gilchrist]

1 minute ago, Corey Hampshire said:

Pardon my ignorance, but where is "Change at Point" located? I see where this could be very powerful and wanted to play around with it, but can't seem to find it.

You must create your chain, with extra "broken endpoints", where you want to make the modifications manually. Chain the Contour path like normal, enter your operation data. Generate the path.

Then, expand the tree for the Operation, click on the "Chain/Geometry Manager". In the Chain Manager, Right-Click on the Chain you want to modify. You'll find "Change at Point" in this right-click menu...

You can do "all kinds of cool things" with Change at Point. You can "jump clamps", you can "turn sections of a path from feed to rapid motion (just be sure to switch back to "feed", you can invoke Canned Text, change spindle speed or feed, enter a Machine or Optional Stop, the list is pretty broad.

This is a function that has been in Mastercam for 20+ years, but very few users are aware of it! I've taught some lessons on how to use it, and modify Canned Text output in the Post, to do some really trick customization...

[Corey Hampshire]

11 minutes ago, Colin Gilchrist said:

You must create your chain, with extra "broken endpoints", where you want to make the modifications manually. Chain the Contour path like normal, enter your operation data. Generate the path.

Then, expand the tree for the Operation, click on the "Chain/Geometry Manager". In the Chain Manager, Right-Click on the Chain you want to modify. You'll find "Change at Point" in this right-click menu...

Very cool. Thanks for sharing. I learned something new today. That makes it a good day.

[Colin Gilchrist]

3 minutes ago, Corey Hampshire said:

Very cool. Thanks for sharing. I learned something new today. That makes it a good day.

 Love it when new learning occurs!

I updated my original response too, with a tiny bit of more info...

[Matthew Hajicek - Singularity]

On 12/13/2022 at 11:45 PM, cncappsjames said:

In "engineer's" favorite corner radii... 1/8 and 1/4... metric tools are your friend. 6mm and 12mm respectively.

Or they'll think 1/32", but round it to .030", so I use a .050" endmill.

[Leon82]

i had one drawing where they dimensioned the center of the .125 radii in the corners of the triangle pockets instead of wall intersections so i couldn't use much of the radius tolerance . i had to use a 6mm endmill for it.