Can I use an arbor in a mill as an extension?

I would like to machine a cable drum with grooves with my 3 axis bridgeport cnc mill. The cable drum needs to be 4.5" deep and 4" diameter. I plan to use a long 1" diameter endmill to clean all of the surfaces and then use a convex 3/32" radius milling cutter to cut the grooves. I don't see any problems in the machining until I get to the final milling where I have to cut the grooves. Being that the cable drum is 4.5" deep, I can't find a cutter that can reach the bottom without hitting the stock with tool holder. The only extension that I've been able to find is a 10" x 1" arbor shaft and then use a 3/32" milling cutter that fits a 1" arbor shaft. I haven't used any type of extension before so I am wondering if it would be safe to use an arbor in this situation. I am only trying to make a 0.060" depth cut in aluminum so it is very light machining, but I figured it would be safest to ask for opinions.

I have found accu hold end mill holder extensions, but the only 2 cutters I have found are 7/8" diameter at the cutter with 1/2" shank, or 2-1/4" cutter diameter around a 1" arbor. the 7/8" cutter shank is only 3" long so I would need an extension and the extensions are 3/4" or 1" diameter (would hit the workpiece).

NMTB 3 Milling Arbors 1" x 1" (LOC945) | Superior Machine & Tool
http://www.jtsmach.com/jtswebshop/Workholding/WH172.asp
3/16" x 2-1/4" x 1" Hole Convex Cutter | DrillsandCutters.com
Accu Hold End Mill Holder Extension Hi Precision 3/32 - 1 Inch Diameter 2.25 to 6.5 Long

I have only used erickson nmtb 30 tool holders in my mill and have a rough understand that I can use other nt/nst tool holders in my mill, but could need additional tools.

I know that I am pushing the limitations of my machine a bit and that a cnc lathe or 4 axis mill are more ideal for my project, but if my machine can do it, that would be by far the best option since we will most likely need to make several variations of the part.

Any serious help is appreciated.

Still don't have a solution, but this is what I've come up with so far. I don't think the arbor shaft would work becuase the nut holding the cutter on would also hit the workpiece underneath the cutter. Essentially, the cutter has to be the lowest point because the workpiece spirals up like a cone. Any thoughts?

How hard is it to reduce the shank diameter of a high speed steel cutter?

I have found a radius cutter with 1/2" shank and an endmill extension that has 1/4" ID and 1/2" OD. I can't use a wider extension shaft because it would hit the workpiece so I can either buy a 1/2" OD shank cutter and get it cut down to 1/4" OD.
Concave/Convex End Mills | Travers.com


I also found a cutter with 1/4" shank but the teeth look very small.
Convex Radius Milling Cutter 1/4 Shank High Speed Steel 3/32 1/4 Radius, ID 239-

I have several straight shank collet chucks that I use for extensions when I have to reach down deep.

1" shank ER20's, ER32's, and a couple 3/4 shank DA200's.

edit to add: It looks like the standard cutters don't give you reduced shank you need. You could try making an extension out of 3/4" steel and use the 7/8" x 1/2" cutter, put in a set screw and loctite the shank, take baby cuts. You would be right at the limit of the DOC, you might be able to get away with taking the 3/4" extension undersize a little. It's not going to be shit for rigid.

Maybe an I.D. grooving bar in the mill spindle, treat it like a single point thread mill and helical interpolate your groove?

guest said:

I have several straight shank collet chucks that I use for extensions when I have to reach down deep.

1" shank ER20's, ER32's, and a couple 3/4 shank DA200's.

Click to expand...

Appreciate the input. How do the endmills or cutters perform with those extensions? Do you get more vibrations or have to slow down/shallower passes?

I have da180 and da300 collets so one of those extensions would probably be a good addition. The DA300 extension has a 1/2" OD so I still need to find a cutter with 1/4" shank.

I usually use the DA's for drilling or tapping, and the ER's for milling. It works okay, just don't extend more than you have to and don't be aggressive in the cut.

I think the challenge is going to be the diameter of the cutter vs. the diameter of the extension. You might have to have a shank ground down.

It would be worth an email to KEO to find out what a special cutter would cost.

edit to add: This is what I had in mind wrt the ID grooving bar idea

Grooving and Cut-Off

Grooving and Cut-Off

Program it as a 1.375 dia cutter, and run a helical interp. You have a 1" shank so you have some rigidity, and you can use inserts instead of HSS. You could get .150 deep on your groove, and no clearance issues.

I've got one of the smaller top notch bars, I haven't actually tried to run it like this, but I can't think of a reason why it wouldn't work?

swf- I tried out my little top notch bar in my bridgeport this morning. I cut one groove .020" up off the floor, and another cut .200" up from that. One pass .050" DOC conventional cut- piece of cake.

Here's a pic:

edit to add: my bar is A08-NER2 and the insert is NG2058L, so I think the insert you would want is the NRP3094L. (I always get confused on which hand )

I have done beutiful radiused groves in the edge of aluminum knobs with nothing more than a 1/2" CCGT060204 insert in a turning bar a similar way before, not fast, but a finish to damn near die for!

I ran that at 2000 rpm and 10 IPM. Could barely even hear it cut. Finish is beautiful, I could have easily run it at twice the speed.

guest said:

I ran that at 2000 rpm and 10 IPM. Could barely even hear it cut. Finish is beautiful, I could have easily run it at twice the speed.

Click to expand...

Thanks for the input on both threads. Getting a little overwhelmed with ideas and options. What depth can you get with that groove? I need somewhere around .050-.070".

swflcnc said:

Thanks for the input on both threads. Getting a little overwhelmed with ideas and options. What depth can you get with that groove? I need somewhere around .050-.070".

Click to expand...

I linked to the bar and insert you need in post #5. Just make sure the insert is the "L" and not the "R" that I initially posted. The correct insert one is the one I listed in post #6.

It's a 1" shank bar, and your groove can be up to .150" deep. The bar is 12" long, so you can just lop off what you don't need to get your reach, and stick it in a collet. DMin is 1-3/8, so you would program is as a 1.375" diameter cutter. It will work much better than one of those key cutters- you are not dealing with the little 1/4" shank which will snap if you sneeze on it.

Check the links I posted. They show the dimensions and geometry. The test cut I ran this morning was with a 1/2" bar, so it uses a #2 size insert, but the geometry is the same. What you need is the 1" version and the #3 size insert. Check Carbide Depot for better pricing than Kennametal list price.

guest said:

I linked to the bar and insert you need in post #5. Just make sure the insert is the "L" and not the "R" that I initially posted. The correct insert one is the one I listed in post #6.

It's a 1" shank bar, and your groove can be up to .150" deep. The bar is 12" long, so you can just lop off what you don't need to get your reach, and stick it in a collet. DMin is 1-3/8, so you would program is as a 1.375" diameter cutter. It will work much better than one of those key cutters- you are not dealing with the little 1/4" shank which will snap if you sneeze on it.

Check the links I posted. They show the dimensions and geometry. The test cut I ran this morning was with a 1/2" bar, so it uses a #2 size insert, but the geometry is the same. What you need is the 1" version and the #3 size insert. Check Carbide Depot for better pricing than Kennametal list price.

Click to expand...

Alright, so I'm on board with getting a grooving bar and insert. That seems like an even more applicable tool than the keyseat cutter. Definitely more solid of a tool and it seems like a valuable tool for a variety of applications.

Now for 2 more questions:

How much of a difference will I notice in conventional milling vs climb milling? The code will be a lot easier to rewrite if I can do one drum conventional and one climbing.

What would you recommend for the initial cutting of the spiral, before cutting the grooves. The grooving bar and a flat insert to do the first flat pass?

Thanks for the help. I feel like I have found a good solution now. And sorry for any dumb questions. I haven't done a ton of heavy milling in solid steel or aluminum. Mostly just full tool width plunging and cutting in steel plate.

I didn't mean to mix two threads together so please post any additional tool comments on my other thread (Thread: How would you mill a cone from round stock. Indexable face mill or long endmill?)

swflcnc said:

...How much of a difference will I notice in conventional milling vs climb milling? The code will be a lot easier to rewrite if I can do one drum conventional and one climbing.

Click to expand...

I did both on the test cut, no noticeable difference but it's a bridgeport so no ballscrew. Conventional keeps the table from jumping around.

On your machine, on this part-it won't matter.

swflcnc said:

What would you recommend for the initial cutting of the spiral, before cutting the grooves. The grooving bar and a flat insert to do the first flat pass?

Click to expand...

What initial cutting of the spiral? Just cut the groove. Start off the side, feed in to the center and start your helix. Full DOC, one pass. You have a .094 RAD .060 deep. The groove is less than .187 wide. Take a test cut on piece of scrap to get your speeds, but 2800 and 14ipm should be tame.

The trick is going to be getting over the corner and the grooving the chamfer.

Thanks for the reply jancollc,

The initial cutting of the spiral that I was referring to is the last 4 wraps of the wire that will need an inward spiral (not just upward) from a 4" OD to 2" OD, so whatever type of cutter I use would need to cut up to 1" of material away in some number of passes. I don't know if you saw the photo from the other thread but here it is.



I agree with you that I can easily cut the groove in one pass for the upward spiral. I could even cut the inward-upward spiral groove in one pass as well once the flat contour of the upward spiral is milled.

swflcnc said:

...I agree with you that I can easily cut the groove in one pass for the upward spiral. I could even cut the inward-upward spiral groove in one pass as well once the flat contour of the upward spiral is milled.

Click to expand...

You have a cylindrical section and a conical section. You need to finish both before you cut the groove.

What is a very simple toolpath on the lathe is not as simple on the mill, but you need to finish the entire OD before you groove. I would kiss the 4" dia with an end mill to establish the cylinder, and I would have a 2 flute chamfer tool ground to cut the conical section. You don't have to cover the entire conical surface in one pass- just step over and down on the angle. Simple G02 circle on both tools.

Then use the grooving bar to cut the helix. Start at the bottom and wind all the way up, or vice-versa. Grooving the conical section is the trickiest part. As you go up, the diameter gets smaller. So simple G02 XYZ doesn't cut it. That toolpath is a nautilus spiral, you have to divide the circle into sections, or do point to point with a continuous changing rad/arc center. I assume you have adequate CAD/CAM to generate the toolpath.

Sounds good. I will update in a week or so once it is done, or sooner if I run into problems!

Well... It took a little bit more than a week, but here are the finished products. A pair of cable drums.