Parting Line Tips/Tricks??

Nerdlinger · Jun 24, 2016

Please see the attached pic (The part is about 2" tall for reference.) The parts are made in a Speedio and left-to-right progression is: 1) Before Op 10, 2) After Op 10, FLIP, 3) Before Op 20, 4) After Op 20. I try my best to adjust work shifts and keep dimensions tight to minimize the part line but it goes between being smooth to maybe .002". The parting line needs to be small enough to be smoothed out in a rock tumbler...probably something like .0005". I suppose I could probe the hell out of it and get it just about perfect but that would take a ton of time. I am just doing the profile with a 3/8 em. Is there some magical tool I don't know about that is made for this? I bet Brush Research has something but sometimes I dunno about those things...seem kind of iffy to me. Anyone have any ideas?? Thanks!

Booze Daily · Jun 24, 2016

Profile your second side with a ball endmill with your Z depth at the tangent point.

doug925 · Jun 24, 2016

It is always hard to get rid of parting lines. (at least in my experience)
If using a vise, the slight amount of "kick" that lifts the front jaw is enough to change the amount of parting line a few 1/1000's
Once you have the first part machined with a satisfactory part line, put a dial indicator on the part prior to removal.
Insert the next part and tighten the vise until the indicator reads the same zero the original part did.

It's a PITA, but with a little practice, the parting line will go away.

Doug.

doug925 · Jun 24, 2016

Another thought:
Use talon jaws to grip the bottom (excess) 0.06" of stock, and machine the tangs, and the sides all the way down to the talon jaws on Op10. (You will probably want to change to a more robust 5/8 or 3/4" mill with either a relieved neck, or a long LOC.)
Flip the part to a standard vise, and face / drill/ cham the second side as Op20.

Doug.

Captdave · Jun 24, 2016

If a 40 taper machine I would do just as Doug mentioned but Its a 30 taper so bigger / longer tools may not work very well. Screw trying to blend the part line, I would be inclined to lay them down flat with talon grips vise jaws and use HSM paths around the profile and especially the forks, flip and face off the carrier. Yes, it will add one more opt but maybe faster then dealing with the chatter of longer tools.

If you hold the tolerance close then you can gang 6-8 into a vise and do your drilling and may lower your overall cycle time.

Throw it in Cam and check the time, you may be surprised.

Philabuster · Jun 24, 2016

That is not a parting line. I was expecting this to be an injection mold question.

That is a tool blend line between multiple operations.

Captdave · Jun 24, 2016

Was it a cat or feline?

Sorry... Tool blend is more correct.

Comatose · Jun 24, 2016

An automated probing cycle would make quick work of it. Probe for position and rotation, shift the coordinate system and go to town. You already have the probe...

You'd need to use a fairly large probe ball or machine access for the probe in op 1.

Krovvax · Jun 24, 2016

doug925 said:
It is always hard to get rid of parting lines. (at least in my experience)
If using a vise, the slight amount of "kick" that lifts the front jaw is enough to change the amount of parting line a few 1/1000's
Once you have the first part machined with a satisfactory part line, put a dial indicator on the part prior to removal.
Insert the next part and tighten the vise until the indicator reads the same zero the original part did.

It's a PITA, but with a little practice, the parting line will go away.

Doug.

Ive found that using a torque wrench will get the vice always in the same position. Since you put the same amount of force on the movable jaw it is always going to "lift" the same amount so your piece will all be similar. From there you adjust your offset and you can get pretty good result usually a fine sand paper (320 grit or less) will do the job.

Envoyé de mon XT1034 en utilisant Tapatalk

DavidScott · Jun 24, 2016

How much does your machine move during the day? If you don't know then you should.

If your parts are moving then you need to improve the way you are holding it. How do you hold it? We need photos if allowed. If you are not using a torque wrench, or such, to tighten the parts down then start with that. If you don't think it would be worth it at least try it out, torquing your clamp screws will reduce a lot of error if your fixtures are soft.

You shouldn't need to use a ball mill for the last profile. I don't and can maintain a .0002"-.0003" of a mismatch against my stop, never measured it against the vise come to think of it.

Does the mismatch get larger the longer you run the mill or is it random?

Vancbiker · Jun 24, 2016

I try to avoid processing like shown in the OP, but when I have to I'll finish the 1st and 2nd profiles with a ball mill. Blends those mismatches pretty nicely with minimal fuss.

Nerdlinger · Jun 24, 2016

Philabuster said:
That is not a parting line. I was expecting this to be an injection mold question.

That is a tool blend line between multiple operations.

My bad....

Nerdlinger · Jun 24, 2016

Comatose said:
An automated probing cycle would make quick work of it. Probe for position and rotation, shift the coordinate system and go to town. You already have the probe...

You'd need to use a fairly large probe ball or machine access for the probe in op 1.

Yeah, I was going to save that as kind of the last resort...we make thousands of these and all those probe cycles would add up. You're totally right, though...

Nerdlinger · Jun 24, 2016

Krovvax said:
Ive found that using a torque wrench will get the vice always in the same position. Since you put the same amount of force on the movable jaw it is always going to "lift" the same amount so your piece will all be similar. From there you adjust your offset and you can get pretty good result usually a fine sand paper (320 grit or less) will do the job.

Envoyé de mon XT1034 en utilisant Tapatalk

Ha!...I work for a torque wrench manufacturer, so I definitely encourage the use of as many torque wrenches as you can get your hands on

Nerdlinger · Jun 24, 2016

Booze Daily said:
Profile your second side with a ball endmill with your Z depth at the tangent point.

Wait a minute....YEP!...you just blew my mind! Right now I am using a .015 corner rad em so if there is room in Z to use a full rad em it could essentially smooth it out by more than 10X! I'm already doing a finish pass on 10 pcs so the 1.4 sec chip to chip time will add .14 seconds to each part and I can sleep at night knowing that. I've just never run into "TOOL BLEND LINE BETWEEN MULTIPLE OPERATIONS" before, but me thinks this will scratch me right where I itch. Thank you all!

Nerdlinger · Jun 24, 2016

doug925 said:
Another thought:
Use talon jaws to grip the bottom (excess) 0.06" of stock, and machine the tangs, and the sides all the way down to the talon jaws on Op10. (You will probably want to change to a more robust 5/8 or 3/4" mill with either a relieved neck, or a long LOC.)
Flip the part to a standard vise, and face / drill/ cham the second side as Op20.

Doug.

I think using a radius em will work for me but I've never used those talon grips...can they really hold a part by .060" and do a full depth (1.6") profile cut without the part moving? Do you have to baby the tool path or is it as rigid as holding it any other way as long as you have the pressure?

BROTHERFRANK · Jun 24, 2016

Nerdlinger said:
Yeah, I was going to save that as kind of the last resort...we make thousands of these and all those probe cycles would add up. You're totally right, though...

I am curious how long does you probing cycle take to set X,Y and Z work coordinates (3 touch, corner)? The macros we use take about 2 seconds total plus tool change. Not too much to give up to get the mismatch lines minimized.

Bobw · Jun 24, 2016

Blend lines in general suck..

I agree with the torque wrench, and I would also try and run both ops at the same time and
use the same endmill on both ops for finishing. Just eliminates some things from the equoation.

On this part, it seems like you could actually make the blend line look decent. Run your first op deeper,
then run your second op to the depth of the clevis/fork. If you have the tolerance... Run the first op a little
big, and the second op a little small. It'll almost look like its supposed to be there.

Nerdlinger · Jun 24, 2016

BROTHERFRANK said:
I am curious how long does you probing cycle take to set X,Y and Z work coordinates (3 touch, corner)? The macros we use take about 2 seconds total plus tool change. Not too much to give up to get the mismatch lines minimized.

I've got the Renishaw OMP 40 and on other applications I'm guessing it takes probably about 2 seconds per two-touch so I imagine I would need two points in, say, Y and then one more point in X to set the corner as well as any rotation necessary...so 6 seconds per part. 3000 pcs per run would add about 5 hours...so you're right, that's not bad if it works. I'll try using the full rad em on the finish pass first since it adds basically NO time but attack it with the probe if need be.

Nerdlinger · Jun 24, 2016

Bobw said:
Blend lines in general suck..

I agree with the torque wrench, and I would also try and run both ops at the same time and
use the same endmill on both ops for finishing. Just eliminates some things from the equoation.

On this part, it seems like you could actually make the blend line look decent. Run your first op deeper,
then run your second op to the depth of the clevis/fork. If you have the tolerance... Run the first op a little
big, and the second op a little small. It'll almost look like its supposed to be there.

That's plan "C"

Parting Line Tips/Tricks??

Stainless

Titanium

Titanium

Titanium

Titanium

Diamond

Titanium

Titanium

Hot Rolled

Diamond

Diamond

Stainless

Stainless

Stainless

Stainless

Stainless

Stainless

Diamond

Stainless

Stainless

Similar threads