Newbie- Trouble milling hot rolled steel on a manual Bridgeport

[panz]

I picked-up a 1989 series I manual Bridgeport a handful of months ago. My intention was to help me machine parts for a custom loudspeaker I have designed.

Shops in the area would either not quote my parts or wanted in the ballpark of $800 to $2500 to do the work, I figured I could pick up a used mill and learn to do the work myself - saving a significant amount of money in the long run.

The material I am working with is 2" x 6" hot rolled bar stock. An L shaped channel is cut into the workpiece and all sides are faced, my tolerances are fairly wide at +/- 0.010" thus I wasn't too worried about trying this myself.

For one loudspeaker I need to make around 15-20 of these L shaped sections. Each one requires the removal of around 1.75 to 2.5 cu. in. of metal. I started machining with low quality 0.5" HSS tooling, and after several nights learned a few things:

1. The 1/2" diameter endmill would loose its edge in around 45 minutes - if I needed to buy an endmill every 45 min it won't turn-out cheaper to machine this myself
2. I started using 3-in-1 oil as a cutting fluid, turns out I'm allergic to it - my hands turned bright red and swelled-up about 2x their normal size.
3. I estimated 120 machine hours at the current rate I was removing metal.

After this I learned it is possible to not use coolants with many forms of carbide tooling. I did a fair amount of research and found a TMX 1-1/4" indexable carbide insert endmill (directly fits into an R8 taper). The indexable takes APXT-1604 (grade NCM325) inserts designed for steel. This tool worked much better than the HSS tooling I started out with, however I chipped the inserts after running the following settings:

1200 RPM (~400 FPM)
0.020" depth of cut
Feed: somewhere between 10-20 in. / min
Total runtime before edge failure: 1.5 hrs

I indexed the inserts to their second side and found some more tech info on the TMX website and ran the inserts closer to their rated speed:

2200 RPM (~600 FPM)
0.020" depth of cut
Feed: ~ 20 in/min

Now the endmill chatters easily and I'm limited to taking passes at 1/2 width. The mill head makes a bit of noise at this speed, but I don't know if this is normal or unexpected as I don't have anything to compare my mill to. I'm also not sure how much pressure I'm supposed to apply to the cut - do I let the machine do all the work and crank the cross slide just to keep up or do I need to apply constant pressure to keep the chip size right? Did I go down the wrong path with an indexable carbide endmill - should I consider going back to HSS, but how do I solve the sharpening and speed (of metal removal) problem? Is my old bridgeport not up to the task of reliably handling carbide tooling?

Any recommendations for changing my setup, feeds/speeds, tooling, or suggestions for improvements to my machine (just don't tell me I need to rebuild the head) would be greatly appreciated.

-Mark

[little bubba]

A few things, you're limited on HP, you're limited on rigidity. At this point you aren't touching your HP limit. Most indexables, with honed edges on the insert, which you have, will take more HP to move metal, they can beat and bang pretty hard.

With the indexable you have, I would suggest going deep and narrow, instead of shallow and wide(where you can), you will be able to feed faster due to chip thinning (do a search), and use up more of your insert, instead of just the bottom corner.

Having experience trying to make money on floppy machines (your's is), solid carbide vari flute/helix endmills work very well. The trick is to twist the machine up in one direction and keep it that way, narrow and deep to get the head tweaked off to one side, or when slotting(cutting full width), ramp in slowly to tweak the head upwards. Keeps the chatter down and extends your tool life.

[gsrmmeza]

Have you heard the saying? " Stepped over a dollar to pick up a dime!"
You say shops offered to make your parts for $800-$2500.

1: you bought a Bridgeport mill
2: you bought an indexable endmill
3: you had to buy inserts
4: you were running hss cutters that lasted 45 minutes
(120 hours x 60 minutes / 45 minutes = 160 single end endmills or 80 double end endmills )

My question to you is how do you plan to meet your goal of:
"saving a significant amount of money in the long run!"

Also 120 hours / 8 hours per day = 15 days

A suggestion for improvement is to reconsider having them made by one of the shops that quoted the parts.

[mc-motorsports]

Originally Posted by gsrmmeza Have you heard the saying? " Stepped over a dollar to pick up a dime!" You say shops offered to make your parts for $800-$2500. 1: you bought a Bridgeport mill 2: you bought an indexable endmill 3: you had to buy inserts 4: you were running hss cutters that lasted 45 minutes (120 hours x 60 minutes / 45 minutes = 160 single end endmills or 80 double end endmills ) My question to you is how do you plan to meet your goal of: "saving a significant amount of money in the long run!" Also 120 hours / 8 hours per day = 15 days A suggestion for improvement is to reconsider having them made by one of the shops that quoted the parts.

I think that's why he's asking for help.

And I give you points for ambition.
What kind of fixturing are you using?
Post up as much info and pictures as you can and you'll get more response and help.
I would go back to solid carbide endmills, better suited for manual machining mild steel. APXT insertable endmills and facemills are great, but better suited for CNC, more ridgid machines or for conventional milling opps, hard material.

Do you have ballscrews, or acme screws?
And do you know the difference between climb milling and conventional milling?

MC

[panz]

The machine has its original acme leadscrews, in general the sliding surfaces are in good condition. I have been conventional milling with my machine as I've heard the warnings that climb milling with less than perfect machinery is a good way to destroy tooling.

I attached a picture of how the steel is being held in a vise (sitting on parallels). Starting out I was milling each piece individually (less material to screw up - since these were the first things I've machined on a mill). Right now I'm still using the vise, however, I machine a piece of steel around 5 x 6 x 2" into the right form and slice the individual pieces off.

I assume that once you get into the "chatter zone" with a solid carbide endmill it's darn near instantly destroyed? What I don't have a feel for is how far I can push the machine before I should worry about the tooling. When I was looking into mills I seriously considered one of the import manufacturers' RF45 style mills - looking back if the 'Bridgy is considered floppy it's a good thing I didn't try one of those machines.

[Crevice Reamer]

Have you considered using the MUCH MORE EASILY MACHINABLE 12L14 steel?

http://www.speedymetals.com/c-8249-12l14.aspx

CR.

[panz]

Originally Posted by Crevice Reamer Have you considered using the MUCH MORE EASILY MACHINABLE 12L14 steel? http://www.speedymetals.com/c-8249-12l14.aspx CR.

I stocked up on 2x6" hot rolled steel for this project before I found out it was not the ideal material to work with. Originally I wanted to go with 1018 cold rolled, but my local metal supplier wanted a large minimum order to get something they didn't have in stock.

It would be great to get some feedback on the recommended starting ranges (for my manual Bridgeport) for both solid carbide (say a 1/2" endmill) and my 1.25" indexable. I've tried a depth of cut anywhere between 20 thou and 50 thou with varying success depending on the width of cut. However I hear wild claims of people on the 'zone hogging 150 thou off with a 2" indexable endmill on Bridgeport clones and this makes me think I'm doing something very wrong since I can't touch those numbers.

-Mark

[little bubba]

Here are some real #s from a part that I ran on a Wells Index 847, cnc'd but a similar machine. 1/2" carbide variflute probably from lakeshore. 4140 annealed, .800 deep, 2400rpms, 25ipm, .060 width of cut. So.. 1.2cubic inches a minute. 2hp motor and ran into some HP issues as the tool dulled.

As for a full width cut, same endmill, same part, .05 deep, 30ipm.

[RotarySMP]

Are the gibs adjusted right on the dovetails? Are you locking the axis you are not moving?

[panz]

Originally Posted by RotarySMP Are the gibs adjusted right on the dovetails? Are you locking the axis you are not moving?

The gibs are adjusted for a moderate amount of drag while feeding the table. The quill is all the way up and locked, however I don't lock the axis I'm not feeding - does that make a big difference? I noticed my knee doesn't even have a lock lever, there appears to be a brass plug where the locking handle should be.

[mc-motorsports]

Yeah, cold roll is a lot easier to machine. Hot roll is a lot harder.

Try this: 1/2" solid carbide endmill, full DOC, 10-20% step over.

Going with a shallow DOC like that will wipe out the tip of that tool as that's all your using. Using more of the flute and a shallow step-over can increase tool life by removing more material without using the edge so much. At a .050 DOC, your only using 5% of your cutting edge that you paid for. Slow down to around 1000-1200 RPM. A lot of RPM's and feedrates being quoted are for CNC, diffrent story all together.

And yes, some people will refer to a BP as "floppy", but that is comparing to the high end CNC's of today. Night and day difference for sure, so is the price. For sure it is one of the most ridgid knee mills you can buy, an import would be a major step down.

Another thing you might want to do is rig an air line to blow those chips out while your cutting, or use a coolant mister, would help a lot, but the coolant tends to get messy. Either will help a lot.

MC

[panz]

Originally Posted by mc-motorsports Yeah, cold roll is a lot easier to machine. Hot roll is a lot harder. Try this: 1/2" solid carbide endmill, full DOC, 10-20% step over. Going with a shallow DOC like that will wipe out the tip of that tool as that's all your using. Using more of the flute and a shallow step-over can increase tool life by removing more material without using the edge so much. At a .050 DOC, your only using 5% of your cutting edge that you paid for. Slow down to around 1000-1200 RPM. A lot of RPM's and feedrates being quoted are for CNC, diffrent story all together. And yes, some people will refer to a BP as "floppy", but that is comparing to the high end CNC's of today. Night and day difference for sure, so is the price. For sure it is one of the most ridgid knee mills you can buy, an import would be a major step down. Another thing you might want to do is rig an air line to blow those chips out while your cutting, or use a coolant mister, would help a lot, but the coolant tends to get messy. Either will help a lot. MC

MC - Thanks for the feedback. Since I toasted a 1/2" carbide endmill, is it possible to get it resharpened? [I realize the diameter will be smaller - but it doesn't matter to me since I need to take multiple passes anyway] What are the average costs for getting tooling resharpened and do shops even consider it if you only have 1 or 2 endmills for them to process? Is it possible to sharpen endmills yourself or is the equipment extremely expensive?

How would a "corncob" roughing endmill be different from the standard endmills I'm using - does it offer any advantages or do you need high-end equipment to get the performance benefit out of it?

I also noticed my milling vise can separate from the angle base it's on - I'll unbolt the two and zero the vise back in directly on the table. I didn't consider that could be a problem, but I might as well take it out of the equation.

Thank you all for the suggestions