Best Finishing strategy for this part?

[crazy^millman]

nope     threadmill.

 

Okay you threw me off with the way you worded that operation. You meant Threadmill Operation using a Ball endmill, but using that operation to drive the tool. Good solution.

[Müřlıń®]

Ok, I have G17 18 19 on now. Made it alot better. But still about 40k lines of code. Here are my current settings.

 

total tol. =  .010

stepover, distance .005

50/50 cut tol. line/arc tol

min arc rad .5

max arc rad 100

 

the surface finish needs to be 32. and my spindle is max at 3500rpm

 

How to I attach a pic of my desktop screen?

impossible finish on your machine....

If your SS is only 3500, your machine tool is incapable of producing that type of surface finish using a ball/ramp, I am guessing there will be too much slop in the machine tool itself......use high speed waterline and take a flex shaft cable grinder with a hand made star pad and polish it to a +32 finish in 10 min....

 

I use a Haskins 2 hp cable grinder...

[cherokeechief79]

I cut hydraulic 60 deg valve seats in 41 and 4340 pre heat treated steel parts all the time.

the previous machinists who did this job would use 2 custom carbide angle cutters.

they would rough with one and just touch it with the 2nd.the finish had to be 32 and they had to polish the surface with grinding compound and a dremel and a wood dowell with the 60 deg taper on it.

it was an absolute nitemare because the parts weighed in excess of 200 lbs and there were 2 60 deg ports one was only about a 1/4 inch at the top and the other was about .5

if the tool chattered even the slightest they got rejected when QA checked them with a borescope and prussion blueing.

it was almost impossible on the machine to check the finish on the smaller angle.

it was also impossible to pick the hole up again to remachine it once its removed from the machine.

these were round parts laying flat on a hass small horizontal with a built in 4th axis table.

I tried every toolpath possible to get the 32 finish and could not get anyting to pass for a seal surface.

that's when I tried using the threadmill function.

 

the 32 finish was now not a problem without polishing at all (even running at only 3500 rpm with a .125 ball for the smaller hole)

I can use wear offset now and have complete control of the diameter.

its simple to program.

the tol on the angle was 60 deg +.5 so it was simple to program a taper of 60.25 deg.

[Müřlıń®]

I cut hydraulic 60 deg valve seats in 41 and 4340 pre heat treated steel parts all the time.

the previous machinists who did this job would use 2 custom carbide angle cutters.

they would rough with one and just touch it with the 2nd.the finish had to be 32 and they had to polish the surface with grinding compound and a dremel and a wood dowell with the 60 deg taper on it.

it was an absolute nitemare because the parts weighed in excess of 200 lbs and there were 2 60 deg ports one was only about a 1/4 inch at the top and the other was about .5

if the tool chattered even the slightest they got rejected when QA checked them with a borescope and prussion blueing.

it was almost impossible on the machine to check the finish on the smaller angle.

it was also impossible to pick the hole up again to remachine it once its removed from the machine.

these were round parts laying flat on a hass small horizontal with a built in 4th axis table.

I tried every toolpath possible to get the 32 finish and could not get anyting to pass for a seal surface.

that's when I tried using the threadmill function.

 

the 32 finish was now not a problem without polishing at all (even running at only 3500 rpm with a .125 ball for the smaller hole)

I can use wear offset now and have complete control of the diameter.

its simple to program.

the tol on the angle was 60 deg +.5 so it was simple to program a taper of 60.25 deg.

Threadmill is a very elegant solution for your application and I will definitely be using your trick when the time comes  

 

However this part is a 15" oval and he is using a 1" ball.  The amount of machine tool travel is huge...With 3500 RPM it is going to be impossible to keep the tool loaded given the feedrate he is going to use with his machine..

 

So If there is any reversal comp being used in his machine, or any backlash in the ball screws/or way configuration it will make it impossible.

 

I am assuming this  because he only has 3500,  his machine tool is not accurate to .0001 when cutting this oval.

[jlw™]

I only tweaked your file and really liked the way flowline spiral looked. I'd run that first.

[cherokeechief79]

yes you are right. I didn't see that.

the threadmill trick will not work on an oval only round.

[Oppiz]

He's a quick easy way to do this, a basic 2d contour with depth of cut set it to cut a taper. I did this years ago before I had surface. Also this works good for the old machines with little memory.

[cherokeechief79]

He's a quick easy way to do this, a basic 2d contour with depth of cut set it to cut a taper. I did this years ago before I had surface. Also this works good for the old machines with little memory.

I got real excited when I saw this but could not get it to cut continuous.

[cherokeechief79]

why couldn't mc just add a field for angle in the helix bore cycle?

this seems like a simple solution .

 

[JVizzi]

Thank you all for your help. I ended up going with the Flowline toolpath that John helped me with. with a .0001 scallop it came out quite smooth, with a light zipper line. No problem for our Prep department.

 

Thanks again