Welcome to MCAD Central

Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.

Register Log in

Ball nose mill and mill marks?

kumaichi

New member
Hi,


I have a small part that has a chamfer in it that is roughly 4.25mm in length. I did the toolpath, profile with a ball nose end mill and when it completes, the surface is really bad on the part. I figured if I make really small movements in the z axis it would leave a nice machined surface. I'm using a 5/32" 4 flute ball nose end mill, moving in the z direction at 0.15mm each step and have a cut feed of 150mm per minute. The cutter was brand new so I don't think that was the problem. I first rough the path with a 5/32" square end mill and I leave 0.25mm material for the ball nose operation.


Is there anything I can do in the cut path that will leave a better finish on the part? I'm trying to polish the part to a mirror finish and with all these lines in the part, it takes for ever for the tumblers to polish it.


Thanks in advance for any insight.


Have a great day,


Craig
 

tinag

New member
Hi Kumaichi,


Have you tried setting the wall scallop height ? It can be found in the advance parametres.


TinaG
 

kumaichi

New member
Hi Tinag,


Thanks for the quick response. I looked at the help file and it says that if you are to use the wall scallop parameter that it should be set to d/2 which in my case is roughly 2mm. I'm not familiar with this setting,does that mean every slice would move down 2mm in the z axis?


I will give it a try and see if that improves the finish on my chamfer.


Thanks again,


Craig
 

marker4x4

New member
kumaichi said:
Hi Tinag,


Thanks for the quick response. I looked at the help file and
it says that if you are to use the wall scallop parameter that it
should be set to d/2 which in my case is roughly 2mm.


Craig,



Wall scallop parameter is the "depth" of the grooves that your ballmill creates at each consecutive pass.

In the other words, smaller number in there causes tighter toolpath thus better surface. Try 0.01MM ans see what happens.



Also make sure that you use descent RPM speed; it's rather small cutter you're using.


Edited by: marker4x4
 

vishnushankar

New member
hi Craig


Tina is very right when she said that you need to set your wall scallop height. This parameter is very similar to specifing <scallop height>.... as this automatically controls the step over of the tool on a flat surface.


In your case if you specify a smaller wall scallop value like Marker4x4 suggested it would give you a good result but your step depth for each pass gets reduced. So in a nutshell it is a compromise between the machining time and good finish.


It also depends on what type of nc sequence are you creating like volume milling or surface milling.


Regards


Vishnu
 

kumaichi

New member
Thanks marker4x4 and Vishnu for your suggestions. I tried setting the wall scallop to 0.01mm and played the path and it will take 461 slices. At 150mm per minute, that would take a really long time :-(. As Vishnu suggested, it's a trade off between finish and machine time.


I'm currently using a profile sequence to make the cut. Would another type of sequence give me a better finish in a reasonable amount of cut time? I guess it's just a matter of experimenting with wall scallops and nc sequences to find a happy balance.


I attached a photo so you can see my dilema, the outside chamfer is the sequence I'm not getting a very good finish on.


Thanks again for your help with this.


Craig


View attachment 489
 

cncwhiz

New member
Why don't you use a chamfer end mill and just do a few step over's? If the chamfer is the same angle this should be a piece of cake.
 

marker4x4

New member
kumaichi said:
Thanks marker4x4 and Vishnu for your
suggestions. I tried setting the wall scallop to 0.01mm and
played the path and it will take 461 slices.


Craig


I'm not sure how would you end up with 461 slices over 4.5MM distance
????? It would help if you posted a snapshot of your param. window with
all your numbers in it. It's easy to punch numbers in the wrong place
and then everything goes down south.
 

marker4x4

New member
cncwhiz said:
Why don't you use a chamfer end mill and just do a few
step over's? If the chamfer is the same angle this should be a piece of
cake.


That chamfer looks like it's variable angle, but maybe it's just the pic.



Hey Craig, why don't you try Surface Milling instead? Might actually work better for you.
 

tomwalls

New member
cnc whiz is correct in stating that if this chamfer is a constant angle
all around, then having a tool ground to this angle is the most
efficient way of accomplishing this cut. Use a profile sequence, with
the mill surface being a sweep. Make the trajectory of the sweep the
contour of the chamfer (outside shape of the part), and the cross
section starting at the top of the chamfer, and the bottom some
distance (say, .1") away from the side of the part. This will keep the
point of the angled end mill (which has zero diameter) away from the
side of the part contour. The point of an angled end mill doesn't cut
well, due to having nearly zero diameter, so it's best to not involve it
in the cut if possible.

Of course, if this is a one-off part, and/or for some other reason
doesn't justify the cost of having a custom tool ground, then 3D
surfacing is your only alternative. I do this myself quite a bit for one-
off parts, since the trade-off between cycle time and waiting (and
cost) of a custom ground tool is acceptable. If the material is
aluminum, plastic, or some other easily machined material, the cycle
time isn't that bad. If it's steel or something more difficult to
machine, consider investing in a carbide inserted ball end mill.
These can be run at very high speeds and feeds, which will minimize
the impact of a large number of passes. Of course, now we're talking
tool cost again, so you have to decide what's most cost efficient.

"Just my 2 cents worth", but when I'm 3D surface milling with ball
end mills, I use a scallop height on the order of .0005" if I'm not too
concerned about finish, and .00005" if I want a fine finish. With that
setting, you can barely feel the ridges with your fingernail. If you
need to polish, this will minimize the effort required. Something not
stated before: the bigger the ball end mill, the fewer passes will be
generated by a given scallop height. So, use the biggest ball end mill
you can live with in a given situation.

Hope this helps!
 

kumaichi

New member
Wow, thanks for all the input.


The chamfer is a single angle, I think, but I can't figure out what the angle actually is, if it's 45 degrees then I can just buy a chamfer mill like what was suggested. I tried using the Analyze function but can't figure out what I need to select to get that working.


I've attached a screen shot of my params using a wall scallop of 0.01mm. If someone notices something please let me know.


For this project, I don't think having a custom cutter made would be viable, it's a small batch of brackets but I still need to finish them to a polish and probably end up anodizing them as well.


Thanks again for everyones input.


Craig


View attachment 492
 

marker4x4

New member
kumaichi said:
I've attached a screen shot of my params using a wall
scallop of 0.01mm. If someone notices something please let me
know.


Just what I've expected




But in its infinite wisdom, PTC has made the STEP_DEPTH and
WALL_SCALLOP_HEIGHT parameters fight with each other. Basically ProMfg
looks at those two values and selects the smaller one. So what you want
to do is the set STEP_DEPTH at say, .1MM or even 1.0MM. Something
really big compared to the SCALLOP that you're looking for. ProMfg will
then ignore STEP and use only the SCALLOP parameter to create your
toolpath. The funny thing is that you must enter something in the STEP
field, otherwise it will come back asking for it. Go figure.



OTOH this awkwardness has it's good points when you stitch a e.g.
90deg. round going from horizontal to vertical. At some point while
cutter is going incrementally down, the STEP parameter starts to take
over the SCALLOP and prevents the cutter t odrop suddenly by 1/4" or
so.... All the little things we learn the hard way.



Anyway, let us know how it went
 

kumaichi

New member
Well, interestingly enough, I set the Step_Depth to 0.1mm and kept the Scallop at 0.01mm and when I generate the gcode, it's actually moving in the Z axis at 0.1mm, isn't it supposed to move at 0.01mm since the scallop is the smaller number? Now when I run the code, I get 46 slices, this is much better than 461 but now I wonder if it's too big, the step depth anyway.


I took another screen shot of my params with the changes you suggest.


Thanks,


Craig


View attachment 493
 

marker4x4

New member
kumaichi said:
Well, interestingly enough, I set the Step_Depth to
0.1mm and kept the Scallop at 0.01mm and when I generate the gcode,
it's actually moving in the Z axis at 0.1mm,


Well, change is good




I'm not sure where the .1 jump in Z came from - it may be some lead_in
move. It would actually help if you posted the screen shot of the
param. window in ADVANCED mode (just click the ADVANCED button in the
top-right corner of the param. window).



BTW: You can actually see the XYZ coordinates while still in the
sequence: click on CUSTOMIZE, let the toolpath work its way out and
then you can click on any line of text in the CL DATA window and scroll
slowly down with the DOWN arrow key. You will see the silhouette of the
cutter appearing on the path and moving along as you scroll. The
current coordinates are in the highlighted line. This way you don't
have to G-code the whole thing to find out position details.



I hope it helps.
 

kumaichi

New member
That is very cool, thanks for the tip, I'm learning all kinds of new stuff today, it is certainly a good day :).


Below is two screen shots of my advance parameters, couldn't figure out how to do it in one shot, sorry about that.


I feel back taking up so much of your time, I really appreciate your help.


Craig








View attachment 494


View attachment 495
 

Mildfire

New member
kumaichi said:
Well, interestingly enough, I set the Step_Depth to 0.1mm and kept the Scallop at 0.01mm and when I generate the gcode, it's actually moving in the Z axis at 0.1mm, isn't it supposed to move at 0.01mm since the scallop is the smaller number? Now when I run the code, I get 46 slices, this is much better than 461 but now I wonder if it's too big, the step depth anyway.

OK, the reason it is stepping at .1mm is because a .01 scallop on 45 degrees with a 5/32" ball allows for a step down of .28mm. However, I personally don't like using profile milling unless the surfaces are near vertical. This is a perfect part for Cut Line machining.


Try this, create a new sequence, choose surface mill, set your parameters as before using .2mm for stepover and leave scallop height as "-". Now select the surfaces of the chamfer and the surfs below it.


In the Cut Definition menu select Cut Line and then Closed Loops. Hit the green + sign, select the top boundary of the chamfer and accept. Hit done and then OK. Click the + sign again, select the bottom boundary of the part, acceptand hit done and OK. Now in the bottom right corner click the cutting direction icon and toggle which direction you want to machine, accept and hit OK.


This method give a nice clean toolpath that blends between boundary curves and also works with open contours. You get a uniform stepover across the extents of the sufaces for an even finish. You can drive the stepover by scallop height if you want, but I typically don't.


Hope this helps.
 

kumaichi

New member
Thanks everyone for all of your help. I cut one this morning using the Surface method provided by Mildfire and I also purchased a 45 degree chamfer cutter which I will try when I get it.


The surface method worked really well, no lines at all. I think I need to adjust the speed of my feed and maybe the spindle speed, I got kind of a strange texture, almost wavyon the part but I think the tumbler should be able to work that out in no time.


Thanks again to everyone who replied with suggestions, I learned alot from this project.


Have a great weekend,


Craig
 

althezard

New member
When using a ball end mill with a small step depth or scallop height, you can, and probably should, boost your feedrate. The reasoning is simple. As the depth of cut gets shallower, less of the tool is engaged in the part. The chip becomes thinner. Radial force becomes correspondingly less. Tool wear becomes correspondingly greater on the cutting surfaces. I don't have the formula handy, but as a rule of thumb, you can increase the feedrate by an inverse proprtion to the percentage of the cutter radius. For example, if you are using a 10mm tool, the radius is 5mm. If your depth of cut is 2.5mm, you can increase your feedrate by about 100%. If your depth of cut is 1mm, try boosting the feedrate 1000%.
 

cncwhiz

New member
althezard,


What you gain in tool life by your formula might hold true for the contact area, but will not work correctly for finish as that you have exceeded the recomended sfm. And as far as upping your feed rate 1000% most if not all machines can not go that fast in actual feed at the controller level. This type of problem can not be corrected by forumlas but must be done hands on to get the results the you are trying to get. If I buy a 1/2 end mill for twenty dollars and I am concerned about tool life when the person that has to blend the scalops and bad finish away do alot of work to fix the new problem how much money did I save?


 

Sponsor

Top