What causes his "Pock Marked" finish ??

If you are observing "cut lines" the feed rate is too much for the radius of the tool.

Plus the tool may not be correct.

Meaning if you are cutting from right to left the left side of the tool is doing the cutting.

Many may have a pointed tool like a 60 degree thread cutting tool that due to the point they can cut grooves or threads instead of removing material.

Aluminum can be nasty stuff and dawn works wonders but can cause rust.

ATF works very good on lots of things and with it giving a high detergent level cleanup is easy and the machine will be cleaner with ease use and wipe down.

Sent from my SAMSUNG-SGH-I337Z using Tapatalk
 
Greg, which of these tools are you using?

s-l400.jpg

For turning toward the headstock, you should be using the second tool in from the right. The last one on the right is for facing.

I think those inserts are TCMT inserts. If so, they are a triangular positive rake insert with a 7 degree clearance angle. Typically, these inserts are used in steel, not aluminum, although they will work. Do you know what your nose radius is?

I agree that your speed is way too low. Cutting speed for aluminum varies with the source but for carbide inserts, the typical speed is somewhere over 2500 SFM. For a 1.2" OD piece of 6061, you're looking at a spindle rpm of over 10K, which you don't have, so just run at the max speed your lathe will run at. Adjust your feed to the mid-range of what you have available and adjust up or down as needed for a decent finish.

Roughing depths of cut with this insert varies with the insert maker. I have tools that use that insert and know that you can easily take a 0.100" deep roughing cut. Finish depth of cut depends on the nose radius; typically, you can use about 1/2 the nose radius and the insert will cut. For example, if you have a nose radius of 0.008", a finishing depth of cut would be around 0.004" and the insert should cut without deflecting too much.

Looking at your work piece, I am going to guess that your speed is way to slow and your feed is too fast. Your depth of cut is probably okay for a finish cut. I would use WD-40, too.

You might want to look at the SCLCR tool holders that take the more modern CCMT and CCGT inserts. They will work well for you on that 9" lathe but as others have suggested, HSS is also a very good option.
 
GreggC said:
I have zero experience with HSS cutting tools,
Can anyone make a suggestion what to buy ??
Maybe hand hold me and post a link ??
Click to expand...
Not a suggestion on where to buy but a good suggestion on what to read to grind your own HSS cutting tools. Many of us here have taken a lot out of this thread, great reading and the grinding process is explained in such a way that you can’t help but not make a tool that cuts good.
Give it a look!
 
Last edited:
mikey said:
Greg, which of these tools are you using?

View attachment 260919

For turning toward the headstock, you should be using the second tool in from the right. The last one on the right is for facing.

I think those inserts are TCMT inserts. If so, they are a triangular positive rake insert with a 7 degree clearance angle. Typically, these inserts are used in steel, not aluminum, although they will work. Do you know what your nose radius is?

I agree that your speed is way too low. Cutting speed for aluminum varies with the source but for carbide inserts, the typical speed is somewhere over 2500 SFM. For a 1.2" OD piece of 6061, you're looking at a spindle rpm of over 10K, which you don't have, so just run at the max speed your lathe will run at. Adjust your feed to the mid-range of what you have available and adjust up or down as needed for a decent finish.

Roughing depths of cut with this insert varies with the insert maker. I have tools that use that insert and know that you can easily take a 0.100" deep roughing cut. Finish depth of cut depends on the nose radius; typically, you can use about 1/2 the nose radius and the insert will cut. For example, if you have a nose radius of 0.008", a finishing depth of cut would be around 0.004" and the insert should cut without deflecting too much.

Looking at your work piece, I am going to guess that your speed is way to slow and your feed is too fast. Your depth of cut is probably okay for a finish cut. I would use WD-40, too.

You might want to look at the SCLCR tool holders that take the more modern CCMT and CCGT inserts. They will work well for you on that 9" lathe but as others have suggested, HSS is also a very good option.
Click to expand...

Hey Mke,
I am turning from right to left,
I am using the center tool at 90* to the piece, which is straight on, clearly a mistake
after reading Tq60's post and reading what you said about using the second from the right
It clicked, I now understand whats happening, this afternoon I will change the tool.
I don't know the nose radius on my bits, the tool set I bought did not say,
Is there a recommended nose radius for aluminum ??
I need to learn about these CCMT / CCGT inserts, can anyone point me in a good direction for that info ??
 
I have the cheap brazed carbide from Horror fraught and found I get a nice surface with a heavy cut. .01"
 
GreggC said:
Hey Mke,
I am turning from right to left,
I am using the center tool at 90* to the piece, which is straight on, clearly a mistake
after reading Tq60's post and reading what you said about using the second from the right
It clicked, I now understand whats happening, this afternoon I will change the tool.
I don't know the nose radius on my bits, the tool set I bought did not say,
Is there a recommended nose radius for aluminum ??
I need to learn about these CCMT / CCGT inserts, can anyone point me in a good direction for that info ??
Click to expand...

I would suggest you get this tool set from Precision Matthews: http://www.precisionmatthews.com/shop/38-turning-38-boring-tool-set/

This set includes both RH and LH turning tools and a steel boring bar. All tool holders take the same inserts, CCGT for aluminum and CCMT for steels. 5 of each type of insert is included to get you started. The silver colored CCGT inserts are uncoated positive rake inserts that will perform really well in aluminum. I do not know the nose radius of these inserts but PM will probably know. These inserts are common and cheap on ebay and will work well on your Shop Fox 9" lathe.

To use them, use the RH tool to cut toward the chuck and the LH to cut towards the tail stock. The shank of the tool is oriented perpendicular to the work piece and it can both face and turn in this position. You will really like these tools, Gregg.
 
I'm not sure what kind of machine you're using, but .010 sounds more like a finish cut than a heavy cut. To me a heavy cut in aluminum could be as much as .250 per pass. A light pass would be in the .030 to .040 range, and a finish pass would be .010 to .005. Unless you have a rigid machine, sufficient speed, and a sharp tool a pass of .005 or less would more likely be rubbing off material than cutting it off.

As for HSS tools I'm not sure anyone sells them pre profiled, and if they do you can bet they're considerably more expensive than creating your own from a blank.. Generally they're sold as blanks and the person buying them profiles them to the shape they need. You can buy tool blanks individually or by the box from places like Shars, McMaster, Travers, or any number of other tool suppliers. The nice thing about HSS is that you can make them any shape you want with just a bench grinder, belt sander, disk sander, or any other inexpensive grinder using an aluminum oxide wheel. If you need a new profile for a different job you can easily regrind an existing tool rather than have to go buy a new one.

Personally I use HSS more than 80% of the time. I like the fact that I can make a tool and keep it in the drawer for the next job without having to worry about how much it cost. Victor Machinery sells tool blanks for $.81 to $8.55 depending on size. I doubt many hobbyists will be buying 5/8" and 3/4" blanks, so the prices more realistically are between $.90 and $3.60 per blank unless you're buying in volume.

A simple way to remember the difference between RH and LH tooling is that a RH (Right Hand) tool is used when cutting right to left. A LH (Left Hand) tool is used when cutting left to right. The L or the R is the position the cut starts from.
 
GreggC said:
I don't know the nose radius on my bits, the tool set I bought did not say,
Is there a recommended nose radius for aluminum ??
Click to expand...
I have a similar tool set and if the inserts are TCMT21.51, then the radius is 1 or 1/64" ,I am learning about inserts myself but for what it's worth I think this 1/64 is the ideal radius for a small lathe.,another bit of info is ,read the back of your insert package, if says P), M, K, it means it is designed to cut P=Mild steel, M=stainless steel and K=non ferrous/aluminum .
GreggC said:
I need to learn about these CCMT / CCGT inserts, can anyone point me in a good direction for that info ??
Click to expand...
Here is the best explanation posted by our very own [B]swatson144[/B],,
https://www.hobby-machinist.com/threads/inserts-and-cheap-chinese-holders.6302/.


TCMT21.51 1st position is the shape. This cannot change round peg triangular hole.
TCMT2.51 Insert clearance angle C=7° This can be changed depending on what your material needs**** add more later.
TCMT21.51 3rd position is tolerance class. M is pretty low. If you see anything else in this position (unlikely) except U or N it would be an improvement with no real effect.
TCMT21.51 Insert features.T, with hole, one countersink, and chip groove on one rake face. Pretty much can't change this and still get the larger screw to fit.
TCMT21.51 Size in qty of 1/8" 2 in this case because the inscribed circle of the 3/8" holders in our example is 1/4" can't change or the insert will be too big/small for the holders.
TCMT21.51 Thickness in qty of 1/16" x 1.5 or 3/32" changing by .5 +- probably would not make much difference except adjusting the height at the tool post.may be no decimal
TCMT21.51 Corner Radius in qty of 1/64" can (should) be changed. 1 = 1/64" which is pointy. changing to something rounder can offer an improvement in surface finish.
 
On the "Pock Marked", I can't tell from the photo but is it physical deformed or just looks that way? I can see the radial cut marks but can't see what the speckles are.

I have run across some extruded aluminum recently that looks like it has been galvanized when turned. Only seems to occur in the outer skin and goes away further in. Odd stuff, possibly a defect from the foundry.
 
You must log in or register to reply here.
Back
Top