MS16142-R Port Contour Cutter speed and feed

[Handsome Joe]

Hello,

 

I've been asked to program some port contour cutters for one of our horizontal boring mills. MS16142-10R, 12R, 16R, and 24R. They came out of California and the company can't tell me what they should be run at. Does anyone have experience with these type of cutters that could point me in the general direction for speeds and feeds? I've looked on line and can't find anything, searched the forum too. They will be used on A588 and 316 stainless, any info would be greatly appreciated.

 

Thanks

[Panda_Guy]

You didn't mention if they are HSS or Carbide fluted. 

 

Either way, we usually run them with surface footage appropriate for a reamer of whatever material they are.  In other words, low.  They tend to have a lot of contact at the end of the stroke. 

 

Another trick you may want to explore is to define them as custom tools and draw up their shape and put the spotface at "Z zero", since the spotface has to clean up to create the correct form and radii, etc.  Just be careful with your initial planes so the pilot diameter doesn't hit in rapid.

[Handsome Joe]

They are braised carbide 3 flute. Thanks

[crazy^millman]

Dwell at the end for a 1/2 to full second to help the surface finish. If you can model the bigger ports and get some of the meat out of the port it will help tool life, horsepower and over all quality of the part.

 

20 to 45 SFM would be good starting points and feed them slow .0005 to .001 per tooth feed rate. They are doing a lot of work and the last thing you need to do it scrap a part or tear one up thinking you need to break a land speed record. Normally on a part the porting is the last thing so take your time. I always threw them up on a optical comparator and got the tip to spot face distance and programmed based off of that. That number was recorded on the setup sheet. If a new tool was loaded then that difference was accounted foR. Some do like Panda_Guy recommended. I have done it both ways, but problem is someone will forgot to put that difference in a tool offset. Then they crash the machine and tear up a tool and scrap a part. By using the length from the tip and accounting for that in your program then they may scrap a part, but are less likely to crash the machine or tear something up. I always put comments in the operation with M00 to back off the offset and sneak up on it for the setup part and on the setup sheets. Ports can be re cut as many times as need to get the depth correct, but hard to add material back once it has been over cut.

 

HTH

[taperlength]

I'm doing a similar job now.  Tried all speeds and feeds with no luck.  Probably have to mill the spot face with another tool and not even touch it with the port tool.  Some setups just are not rigid enough.

[jlw™]

I didn't look up the mentioned port cutter but in my experience these don't run as good as reamers but will run good and give excellent results. My go-to brand for port tools is scientific:

 

http://sct-usa.com/products/port-tools/

 

Also, in my experience pilot hole matters, a lot.

[gcode]

I've been doing these ports in inconel lately and have had good luck running

porting tools with no pilots.

I think we get them from Tosco??

[taperlength]

I'm using a SCT with reamer pilot and it works great until the spot face makes full contact then chatters.  So I circle milled the spot face first and backed off the port tool a thou so it does not touch the face.  It's one of those bargain machining centers, sigh.

[Zoffen]

One fun thing i have done is make a custom drilling macro for doing porting tools is a multi parameter drill combo cycle such as:

 

1. Drill to certain depth from finish depth with a R1 Speed and Feed 

2. Now Drill with a "chipbreak style" cycle from here with Q peck and R2 Speed and Feed to a certain depth from finish depth. I usually do this where the seal area is starting to cut to get it not to ratsnest.

3. From here use F1 Feeds and Speeds to Depth with a Dwell if you want.

 

I use this for finishers mostly.

 

Set this up as a custom drill cycle in mastercam. Import operations for all of the cavities you use with your proven speeds and feeds and get good parts all the time everytime. I have done 1000's of these features with very few problems and very solid process stability. Add an M04 at a few thousand RPM to knock any chips off between holes. If the spindle accels/decels fast the g's will whip alot of the chips off of there if any get stuck.

 

HTH!

[The Cathedral]

I get the best results in any material by feeding in slowly like everyone else suggested, then with about .0005 to go I pull back ten thou, drop the RPM to 50, then finish the last half thou and dwell for one second. Of course you have to make sure your infeed method works with your material because if you cause chatter or or working with a gummy material that galls, you'll destroy the finish before you even have a chance.

[Zoober]

Easy peasy. I've done hundreds of ports in valve bodies that require good finishes.

Prep the port by surface contouring the port. That will allow you to leave .003-.005 on all surfaces, including the angles equally. Key is equal amount on ALL surfaces, not just roughing the bore.

Then finish as Ron says, with low surface footage, and .0005-.001 chip load 1/2 second dwell at bottom, unless you get chatter, then in and out, or stop and reverse the spindle and get out. That will burnish a seal surface if needed.

Edit: No pilot needed when equal material is left. there is not enough tool pressure to make the tool bounce.