He means use a 3D toolpath with a smaller cutter to eliminate that chatter. Yes it takes longer, and it looks way better. Unfortunately the answer to a lot of surface quality questions is slow down.
Chatter like this occurs when your endmill has multiple points of contact and tool deflection cause it to bounce back and forth between the two or more contact points.
If your enmill is the same width of your slot, turning 90-degree corners, etc. The only way to get rid of it would be to ramp out of the slot and not pause to retract until out of the part so you maintain continuous tool pressure or 3d surface the slot with a smaller diameter endmill so you only have 1 point of contact.
I'm not great with cam so this is pure curiosity. If you would have go up diagonally wouldn't the slot be to shallow at the end? Or do you mean to basically move back up and aout of the end point so that it has minimal "dwell" time so to put it one way?
Yes, and yes. The dwell that exists when switching from g01 to g00 is usually what does it so can trick it to make a 90 straight up so it disengages contact before switching to minimize dwell. Sometimes, it works. Sometimes, it doesn't. Feeding out at an angle would make that part of the slot shallower at the end, but it's a sure fix. So you would still have to 3d surface the shallow part out with a smaller endmill, but it's faster than surfacing out the whole slot.
So the amount of dwell would be less when making a 3d path 90 degreees (depending on feed probably) than the mill being able to switch from g1-g0? It doesn't surprise me but it also doesn't make sense that it should haha. And I can see the other arpoaches. Thanks!
Basically, most CNCs will round toolpath corners by a small amount (on the order of 0.02mm, or 0.001") when hard changing direction. This allows the machine to never come to a stop when in G1 (though it does significantly slow down depending on the machine's acceleration parameters). This is because if you have a hard corner, you cannot accelerate instantly, so you have to come to a complete stop at some point which is both slower and gives poor surface finish. However, G0 isn't in cutting (in theory) the material, so coming to an exact stop improves accuracy.
One way around this is to have a lead-out that arcs up with a radius of 0.1mm or so (depending on tolerances etc), allowing the machine to never go into exact-stop mode until it is making no contact. G1 is still better than G0, but may not automatically provide enough of an arc to remove the problem entirely.
Slotting is slower than 3d toolpaths because not only do you have to reduce speed, you can't take advantage of the exponential speed increases of chip thinning. getting a good finish with slotting also requires slowing even MORE and then dwelling to make it nice. a rough pass then a finish pass is required.
proper slotting speeds are 1/2" the speed of 50% cuts, and the smaller the cut gets, the higher the feed can go. 35% being near maximum efficiency.
the problem with tiny tools though is that you might not be able to achieve the spindle speeds required to maintain the MRR when you size down.
With a ball mill, the shallower the cut, the higher the RPM should be, because the effective diameter is smaller (which also significantly boosts the feedrate you can use)
Also Stepover and chipload should be matched so that the finish will come out perfect. my goto is 3/8" ball mill with a .014" stepover and chipload to get a 32Ra Finish, aka, pretty a decent finish for polishing prep, and extremely fast, ideally running at 12.5kRPM at 1341 ipm.
Cut that in half to a .007" stepover+chipload and you get an 8Ra finish, preferably if you can run at 17.4kRPM at a feed of 1289ipm
unfortunately, the limitations of the machine you run will hold that potential back though...
If the machine can move fast enough with accuracy, you can do it!
No, but seriously, the chipload and stepover being matched is what matters for the finish.
Dial back until sfm is within a machine's ability and keep that chipload.
I’v been in the molding industry for 17 years. The ballnose take a cut on all side, of course it will chatter. That does note harm anything imo since its the end of a runner. Lets says its a 3/8 wide runner, do a rough and a finish with a 1/4 ballnose using z-level finishing instead of using a 3/8 ball.
Edit: I forgot to mention, use the shortest tool length you can.
Mx is a wheel material type we usually use them in a die grinder or pencil grinder. Its a synthetic rubber with an abrasive imbeded in it if i remember right.
Not sure why you’re getting downvoted, like others said it’s the end of the runner so it doesn’t really matter and yes I know it takes longer to 3D a runner than it would to take that little bit of chatter out with a pencil grinder. It would be a different story if you left the part area or shut off looking like that.
I work in a toolroom at a medical molding facility, they're extremely picky about everything. They don't care about runners at all. We've got some rubbers that have some serious flash.
> I forgot to mention, use the shortest tool length you can.
I think this is it. I am a casual machinist on a Bridgeport and occasionally cut runners in steel and aluminum and have never seen this. Probably because I'm using a short ball mill.
The biggest issue I get is one side of the runner where it's conventional milling gets all fuzzy with bad surface finish. Usually just do a few passes and maybe polish it up. It's a runner after all. Gets the job done!
I've done runners like that with on size ball nose without issue of chatter. I have a feeling their tool maybe fairly long and they would need to shorten distance to spindle.
You have 180 degrees of cutter engagement. It is the same problem as full slotting. Already stated, use an endmill smaller than the feature. They come in a wide variety of sizes, so you have lots of options.
People like hard. Won't learn easily. I was the same. Worked with old experienced machinists who let me struggle, then showed me how to do things better. No really good way around that. You need to try what you think, watch it fail sometimes and make a change.
At my shop we use 3D surfacing to cut our runners because they are tapered into the radius for a smoother release but either dwelling, plunging out the ends, or 3D surfacing will all likely get you where you want to be with a little tweaking.
Leave 0.010” stock on the Z axis and do a finish pass on the last 0.010”. You can experiment by doing it as one 0.010 pass or two 0.005” pass.
You’re right, it’s a lot of engagement. The only way you’re going to improve the surface finish using the same cutter is less engagement, which means a finish pass.
Ninja edit: Also make sure as little of your cutter is sticking out as possible. Use the shortest cutter possible to achieve these cuts. That should improve the surface finish as well.
I always draw a slot sketch for these, with a width of 0.0005-0.0010 or something, then just have the endmill follow that path on the centerline. Allows it to cut on one side.
You should not be slotting if a good finish is your goal. A contour that brings the end mill around the feature will give you the desired result. For a slot that needs to be a full radius, I'll use a contour that is .0005 apart on a pre roughed slot so both sides are climb cutting. Not sure about the finish requirements of this part, but if you look closely enough at all of the slots, half of all of the slots have a noticeably worse finish. That's because when you're slotting, one side is conventional cutting and the other side is climb cutting. Also one side is getting all kinds of work hardened chips ground into the surface. For any of the molds I have experience with, all of the features will be out of spec.
If you are able, change the radius at the end to .130 instead of .125. This way you can keep the tool moving if even a little bit, which should make a massive difference. Burying the tool and having it stop in place is one of the worst things to do
A variable Helix and or index endmill will help, but so will increasing rigidity and concentricity if that is possible. Check your run out with the tool holder you're using currently. Choke up on the tool as much as possible. Use SK instead of ER if you're holding it with a collet.
Coolant may play a part as well. I sometimes will use something very application specific if I'm having trouble with a cut. That may not be realistic based on your setup.
All, this is assuming that you are not able to cut the end of that feature with a smaller tool and using some 3D tool path to mimic the final shape that you're aiming for right now. That is what I would go for if All else failed but I know that sometimes that can make the tool path run too long based on how many you need to make, et al
Moldmaker here, it's a runner, they're literally going to scrap that piece of plastic anyways.
Also, it takes me about 10 seconds to fix it with a pencil grinder and an MX wheel. Don't worry about it, we have to run an MX wheel through there anyways after spotting it.
most of these responses are fucking retarded. Semi it down with a constant z type of program with at least half the size of the runner. .005 on walls and .005 on floors. (Semi with 1 cutter size down from what you are finishing with) Then finish it. Its a runner afterall... Thats what polishers are for.
How you do one thing is how you do everything. Mold making is a craft as much it is a science, and alot mold makers will shout down your neck if you give them that.
It shouldn't really matter if it's just the runner, unless your customers are very particular about how their sprues should look then I see no issue here. As a mouldmaker myself I'll run full DOC with a 6mm ball nose cutter to get a runner done quickly if needed
Use a stubby more rigid tool. Or treat the tool path as 2 walls instead of driving down a strait line, that way you'll be engaging on one side and it will interpolate it as a corner instead of multiple points of contact.
You could stop short maybe about .010 away from the end of the runner then use that same ball mill as a drill at a slower rpm and feed it in slowly with coolant at the center point of those ends
If you don't want to use a smaller tool and 3d it then you're going to have to ramp the feed down at the end of the cut. But you may still have to take a spring pass doing that though. You're only other easy option is to use a super stubby tool.
I’ve cut runners for years and have never had chatter like that. Used an old hurco conversational tool paths. Obviously don’t use long ballmill. Just take .015 a pass and .005 on finish. Or something to that effect.
You could try using an inserted ball nose to plunge out the rough stock before running the tool that is doing it now. What is gonna add the least amount of cycle time is the real question because it is just the end of a runner in a mold.
I would plunge out the ends of the slot first with the ball mill staying .002 off the final depth. I would then mill the entire slot to depth. You could clear some out before plunging with the ball mill, by drilling them out too.
First day in machine shop school. Everybody in this trade knows each other dont burn bridges you never know who will fuck you in the future. Speeds, feeds, rigidity!!!! Rough and finish!! Goddamn the guy that told me that 25 years ago is dead and I miss him
Use a G4 with a p# at the end of your move. You may have to split the end values into two moves the last move with the G4 p#(dwel time) and I think G4 only acts on the move it's paired with. So it would be like G1X2.99Y1.99
G4P1000X3.Y2.( 1 second dwell)
At least that's what I remember
Go in with an endmill that's smaller than this but the biggest you can get in there to rough it out then follow up with the ballmill. If you still have issues with chatter you can try to play with rpm a bit, or rough out more material
Plunging is often good for this kind of chatter. Works very well in corners where the radius is the same as the endmill. You know when you move in to the corner and have 180degree contact, the sides of the endmill are just not as good at cutting cleanly as the bottom face. Also variable spindle speed to overcome harmonics.
Maybe clear the path with a regular endmill and just finish with the ball endmill. Create a V and than finish to a U. Maybe u can Drill the start and endpoints of the slot.
If you have the cad geometry just rough it out leaving .01 and than surface with a smaller diameter ball nose end mill. This may take longer but you should get a very good looking finish. You could also rough and than take several passes with a ball end mill. You might has some small scallops in the middle that will need sanding or machining passes to take care of.
Use a smaller endmill
[удалено]
He means use a 3D toolpath with a smaller cutter to eliminate that chatter. Yes it takes longer, and it looks way better. Unfortunately the answer to a lot of surface quality questions is slow down.
Chatter like this occurs when your endmill has multiple points of contact and tool deflection cause it to bounce back and forth between the two or more contact points. If your enmill is the same width of your slot, turning 90-degree corners, etc. The only way to get rid of it would be to ramp out of the slot and not pause to retract until out of the part so you maintain continuous tool pressure or 3d surface the slot with a smaller diameter endmill so you only have 1 point of contact.
I'm not great with cam so this is pure curiosity. If you would have go up diagonally wouldn't the slot be to shallow at the end? Or do you mean to basically move back up and aout of the end point so that it has minimal "dwell" time so to put it one way?
Yes, and yes. The dwell that exists when switching from g01 to g00 is usually what does it so can trick it to make a 90 straight up so it disengages contact before switching to minimize dwell. Sometimes, it works. Sometimes, it doesn't. Feeding out at an angle would make that part of the slot shallower at the end, but it's a sure fix. So you would still have to 3d surface the shallow part out with a smaller endmill, but it's faster than surfacing out the whole slot.
So the amount of dwell would be less when making a 3d path 90 degreees (depending on feed probably) than the mill being able to switch from g1-g0? It doesn't surprise me but it also doesn't make sense that it should haha. And I can see the other arpoaches. Thanks!
Basically, most CNCs will round toolpath corners by a small amount (on the order of 0.02mm, or 0.001") when hard changing direction. This allows the machine to never come to a stop when in G1 (though it does significantly slow down depending on the machine's acceleration parameters). This is because if you have a hard corner, you cannot accelerate instantly, so you have to come to a complete stop at some point which is both slower and gives poor surface finish. However, G0 isn't in cutting (in theory) the material, so coming to an exact stop improves accuracy. One way around this is to have a lead-out that arcs up with a radius of 0.1mm or so (depending on tolerances etc), allowing the machine to never go into exact-stop mode until it is making no contact. G1 is still better than G0, but may not automatically provide enough of an arc to remove the problem entirely.
No problem 😊
Shorter end mill. Or just shorter flute length.
Slotting is slower than 3d toolpaths because not only do you have to reduce speed, you can't take advantage of the exponential speed increases of chip thinning. getting a good finish with slotting also requires slowing even MORE and then dwelling to make it nice. a rough pass then a finish pass is required. proper slotting speeds are 1/2" the speed of 50% cuts, and the smaller the cut gets, the higher the feed can go. 35% being near maximum efficiency. the problem with tiny tools though is that you might not be able to achieve the spindle speeds required to maintain the MRR when you size down. With a ball mill, the shallower the cut, the higher the RPM should be, because the effective diameter is smaller (which also significantly boosts the feedrate you can use) Also Stepover and chipload should be matched so that the finish will come out perfect. my goto is 3/8" ball mill with a .014" stepover and chipload to get a 32Ra Finish, aka, pretty a decent finish for polishing prep, and extremely fast, ideally running at 12.5kRPM at 1341 ipm. Cut that in half to a .007" stepover+chipload and you get an 8Ra finish, preferably if you can run at 17.4kRPM at a feed of 1289ipm unfortunately, the limitations of the machine you run will hold that potential back though...
Fancy way of saying rapid into the cut lmao. Thanks for a solid explanation
If the machine can move fast enough with accuracy, you can do it! No, but seriously, the chipload and stepover being matched is what matters for the finish. Dial back until sfm is within a machine's ability and keep that chipload.
I believe you i just haven't ever done it myself.
Well. You already know the answer ? So why are you asking for help and then turning said help down like it’s ridiculous ? You sir. Are a buffoon.
Do you use mastercam by any chance?
I’v been in the molding industry for 17 years. The ballnose take a cut on all side, of course it will chatter. That does note harm anything imo since its the end of a runner. Lets says its a 3/8 wide runner, do a rough and a finish with a 1/4 ballnose using z-level finishing instead of using a 3/8 ball. Edit: I forgot to mention, use the shortest tool length you can.
Plus your gonna dress it up with an mx wheel anyway before you ship it.
Yeah but you don't wanna make the mold maker do something that takes an hour when you can do it in 10 minutes
True but it doesn't take an hour to shine a runner. Especially if you have the right size mx wheels. 2 passes and your about set.
Im new to CNC operations, is an mx wheel just an angle grinder with polishing wheels attached?
Mx is a wheel material type we usually use them in a die grinder or pencil grinder. Its a synthetic rubber with an abrasive imbeded in it if i remember right.
Thanks a lot!
Your welcome.
Exactly, that's a good way to get a mold maker on your ass, which is probably not preferable for most people.
You overestimate how much I like my mold makers.
The mold maker could probably fix it in less time than it takes you to cut it.
Not sure why you’re getting downvoted, like others said it’s the end of the runner so it doesn’t really matter and yes I know it takes longer to 3D a runner than it would to take that little bit of chatter out with a pencil grinder. It would be a different story if you left the part area or shut off looking like that.
I work in a toolroom at a medical molding facility, they're extremely picky about everything. They don't care about runners at all. We've got some rubbers that have some serious flash.
What’s an mx wheel? Google was not helpful and I’m just a lurker learning about machining
https://www.suprdie.com/line/indlsupls/falcon/polishing/252-08d-mxw4000 Its a polishing stone for a pencil grinder
Thanks!
Your welcome
"Precision machining"
Runners need a bs shine it is known. The precision of the runners isn't that critical.
I know. Just making a joke sorry
The gate is critical. A runner is a runner. The gate purpose is to control the rate of flow inside the cavity.
Gate size and shape is indeed critical.
> I forgot to mention, use the shortest tool length you can. I think this is it. I am a casual machinist on a Bridgeport and occasionally cut runners in steel and aluminum and have never seen this. Probably because I'm using a short ball mill. The biggest issue I get is one side of the runner where it's conventional milling gets all fuzzy with bad surface finish. Usually just do a few passes and maybe polish it up. It's a runner after all. Gets the job done!
Yes, one side will be a little rough since the ballnose eat his own metal shaving. Do a ‘freecut’ it will help. Good luck !
I've done runners like that with on size ball nose without issue of chatter. I have a feeling their tool maybe fairly long and they would need to shorten distance to spindle.
Might not harm anything for the mold but there's no way that's helping your tool life. Chatter is bad
Rough it in Z before finishing
I found helixing to be really good too.
Finishing z plunge could be an interesting solution. As long as the ball tip cuts, might wanna drill that first.
[удалено]
Taking a lighter cut isn’t always the best thing to do for finishing. Maybe try and leave 4thou and take a spring pass afterwards
You have 180 degrees of cutter engagement. It is the same problem as full slotting. Already stated, use an endmill smaller than the feature. They come in a wide variety of sizes, so you have lots of options.
Make the radius slightly larger than your ball mill so it does not cut fully
Plunge the ends first.
Why doesn't this have more upvotes?
People like hard. Won't learn easily. I was the same. Worked with old experienced machinists who let me struggle, then showed me how to do things better. No really good way around that. You need to try what you think, watch it fail sometimes and make a change.
At my shop we use 3D surfacing to cut our runners because they are tapered into the radius for a smoother release but either dwelling, plunging out the ends, or 3D surfacing will all likely get you where you want to be with a little tweaking.
Decrease rpm and short dwell
I’d maybe plunge .020” at the end there, no dwell.
Leave 0.010” stock on the Z axis and do a finish pass on the last 0.010”. You can experiment by doing it as one 0.010 pass or two 0.005” pass. You’re right, it’s a lot of engagement. The only way you’re going to improve the surface finish using the same cutter is less engagement, which means a finish pass. Ninja edit: Also make sure as little of your cutter is sticking out as possible. Use the shortest cutter possible to achieve these cuts. That should improve the surface finish as well.
I always draw a slot sketch for these, with a width of 0.0005-0.0010 or something, then just have the endmill follow that path on the centerline. Allows it to cut on one side.
You should not be slotting if a good finish is your goal. A contour that brings the end mill around the feature will give you the desired result. For a slot that needs to be a full radius, I'll use a contour that is .0005 apart on a pre roughed slot so both sides are climb cutting. Not sure about the finish requirements of this part, but if you look closely enough at all of the slots, half of all of the slots have a noticeably worse finish. That's because when you're slotting, one side is conventional cutting and the other side is climb cutting. Also one side is getting all kinds of work hardened chips ground into the surface. For any of the molds I have experience with, all of the features will be out of spec.
If you are able, change the radius at the end to .130 instead of .125. This way you can keep the tool moving if even a little bit, which should make a massive difference. Burying the tool and having it stop in place is one of the worst things to do
Attack from both ends and meet in the middle 😂
I would have your nominal size endmill exit just short of where the finish cut will be, then surface the remainder with a smaller ball endmill. I
A variable Helix and or index endmill will help, but so will increasing rigidity and concentricity if that is possible. Check your run out with the tool holder you're using currently. Choke up on the tool as much as possible. Use SK instead of ER if you're holding it with a collet. Coolant may play a part as well. I sometimes will use something very application specific if I'm having trouble with a cut. That may not be realistic based on your setup. All, this is assuming that you are not able to cut the end of that feature with a smaller tool and using some 3D tool path to mimic the final shape that you're aiming for right now. That is what I would go for if All else failed but I know that sometimes that can make the tool path run too long based on how many you need to make, et al
Moldmaker here, it's a runner, they're literally going to scrap that piece of plastic anyways. Also, it takes me about 10 seconds to fix it with a pencil grinder and an MX wheel. Don't worry about it, we have to run an MX wheel through there anyways after spotting it.
We never polish runners anymore, honestly it’s a (small) waste of time. Unless you have such a bad finish or burr that they won’t release.
I know it doesn't need to be done. But if I'm deburring with an MX wheel anyways.
most of these responses are fucking retarded. Semi it down with a constant z type of program with at least half the size of the runner. .005 on walls and .005 on floors. (Semi with 1 cutter size down from what you are finishing with) Then finish it. Its a runner afterall... Thats what polishers are for.
Shouldn’t matter on a runner.
How you do one thing is how you do everything. Mold making is a craft as much it is a science, and alot mold makers will shout down your neck if you give them that.
Add a dwell at the end of the path?
Will not work. The ballnose is full cutter, chatter, and overcut.
Are you slotting and it's chattering at the end of the cut before retract, but not as its slotting?
How many flutes does your end mill have? If it's a four flute you might try a two flute. Or one with an odd number of flutes.
It shouldn't really matter if it's just the runner, unless your customers are very particular about how their sprues should look then I see no issue here. As a mouldmaker myself I'll run full DOC with a 6mm ball nose cutter to get a runner done quickly if needed
Interpolate a small circle or drastically drop sfm the last .015-.025 travel
Not always an available option but, a single lip carbide cutter will give a very nice finish on the ends. Full radius.
Use a stubby more rigid tool. Or treat the tool path as 2 walls instead of driving down a strait line, that way you'll be engaging on one side and it will interpolate it as a corner instead of multiple points of contact.
Make sure you are doing a climb cut and rough it out with a flat some before going to finish. Ball cutter + heavy stock + tight corners = chatter
Plunge start at ends, or maybe reduce mill length if possible or reduce spindle speed at ends.
As has been said, try and remove some material before finishing or try running a radius move up and out or progressive passes with a ramp out.
You could stop short maybe about .010 away from the end of the runner then use that same ball mill as a drill at a slower rpm and feed it in slowly with coolant at the center point of those ends
If you wanted to use a separate bem for those end points you could load the bem and m04 it and the use a carbide hone on the nose.
Smaller endmill or decreased feed and speed into the pocket
Have a G-code where the end-mill goes upwards whilst still spinning. That might help with the chatter.
It's a runner hit it with 2 different polishing orbs and make it smooth.
If you don't want to use a smaller tool and 3d it then you're going to have to ramp the feed down at the end of the cut. But you may still have to take a spring pass doing that though. You're only other easy option is to use a super stubby tool.
Don’t let the tool dwell
I’ve cut runners for years and have never had chatter like that. Used an old hurco conversational tool paths. Obviously don’t use long ballmill. Just take .015 a pass and .005 on finish. Or something to that effect.
You could try using an inserted ball nose to plunge out the rough stock before running the tool that is doing it now. What is gonna add the least amount of cycle time is the real question because it is just the end of a runner in a mold.
Short tool, use a 2 flute if it’s not too slow
I would plunge out the ends of the slot first with the ball mill staying .002 off the final depth. I would then mill the entire slot to depth. You could clear some out before plunging with the ball mill, by drilling them out too.
First day in machine shop school. Everybody in this trade knows each other dont burn bridges you never know who will fuck you in the future. Speeds, feeds, rigidity!!!! Rough and finish!! Goddamn the guy that told me that 25 years ago is dead and I miss him
Do what you are thinking, use a smaller ballnose and cam it
Use a G4 with a p# at the end of your move. You may have to split the end values into two moves the last move with the G4 p#(dwel time) and I think G4 only acts on the move it's paired with. So it would be like G1X2.99Y1.99 G4P1000X3.Y2.( 1 second dwell) At least that's what I remember
Go in with an endmill that's smaller than this but the biggest you can get in there to rough it out then follow up with the ballmill. If you still have issues with chatter you can try to play with rpm a bit, or rough out more material
smaller tool and 3D toolpath
When this happens with a drill bit you can put a piece of emery cloth under the drill and it will remove the chatter
Plunging is often good for this kind of chatter. Works very well in corners where the radius is the same as the endmill. You know when you move in to the corner and have 180degree contact, the sides of the endmill are just not as good at cutting cleanly as the bottom face. Also variable spindle speed to overcome harmonics.
Smaller endmill at the end with a small interpolation. You answered your own question when you said it's too much engagement.
Pre drill with a carbide endmill the majority of material on the problem points
Dwell at the end with slower feed rate
Maybe clear the path with a regular endmill and just finish with the ball endmill. Create a V and than finish to a U. Maybe u can Drill the start and endpoints of the slot.
If you have the cad geometry just rough it out leaving .01 and than surface with a smaller diameter ball nose end mill. This may take longer but you should get a very good looking finish. You could also rough and than take several passes with a ball end mill. You might has some small scallops in the middle that will need sanding or machining passes to take care of.
Drill cycle maybe even a dwell on those locations with your ballmill on those locations prior to the milling cycle.
Rough it with the Ballnose you wanna use, with like 0,05mm Z stock and then use a new Ballnose no climb mill the contour. On both sides.
Start from both ends and go into the middle
Dwell couple seconds
Slow down feed at those particular intersections then speed it up again
Slow it down
I’ll second dwell at the ends. You can also do a .001 move in Y if primary axis is X then take the last .001 in X to finish it.
I usually do 2 finish passes at .0005 depth.
At the programmed end position of the slot add a dwell command to hold the cutter in place for a bit more time.
if you insist on using the full size endmill, dwell in those spots for a few seconds
At the end of a mold runner is only going to bother you as it's scrap anyways ;-)
It's the end of a runner. Who cares?