[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]

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]

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]

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]

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

[mc-motorsports]

You can have them resharpened, but most shops don't want to just do one or two. I don't have endmills resharpened, but a couple of my customers and suppliers do, and they have them done by a small shop which is basically a retired tool grinder who works part time, pretty much 1/2 the cost of a new EM, so for your 1/2" solid carbide, about $7 for a single end.

"corn cob" roughers reduce chatter letting you take heavier feeds and DOC, but the trade off is a bad finish. Not a bad idea, but for what your doing, I would just use a standard 4 flute carbide EM.

And yeah, make your set-up as ridgid as possible. Usually the indexing base of a milling vice is flimsy.

MC

[panz]

Is there such a thing as a high hardness or high tensile strength hot rolled steel? I'm under the (mistaken?) assumption that all hot rolled steel was soft, gummy and relatively easy to work with. When I picked up the steel I am using from the local steel supplier it was in the cutoff room under the pile "hot rolled steel". Is there an easy way to test the hardness of the steel I have to know what it really is? My next step is to shop around locally to see if I can find some CR 1018 so I know for sure what I'm cutting.

[mc-motorsports]

I hope someone has a definate answer to that question, but from my experience, it can go from a little harder than 1018 to almost SS. It's almost like 1020 is not regulated, I quit using 1020 for this very reason, and it's not my imagination. Over 5 years, I've seen it all, and I used to buy enough of it that I would watch the changes in the diffrent shipments that my supplier would get. Use cold roll, it's the cheapest alternative. Free machining alloys are great, but expensive. 1018 is the most reasonable solution.

MC

[Andre' B]

Is there such a thing as a high hardness or high tensile strength hot rolled steel? I'm under the (mistaken?) assumption that all hot rolled steel was soft, gummy and relatively easy to work with. When I picked up the steel I am using from the local steel supplier it was in the cutoff room under the pile "hot rolled steel". Is there an easy way to test the hardness of the steel I have to know what it really is? My next step is to shop around locally to see if I can find some CR 1018 so I know for sure what I'm cutting.

Hot rolled or cold rolled is the process used to form the steel into usefull shapes, you can get 1018 HR or 1018 CR.
If all you know about a bar of steel is that it is hot rolled it could be anything from 1018 to the most difficult to machine mold & die steel you ever imagined.

[JWB_Machining]

Testing hardness is incredibly easy, the catch is you have to have a hardness tester. I'd try contacting your steel supplier to see if they have one, if not maybe contact your local university's engineering deptartment or look for material engineering firms in your area. Even try some of the shops in the area they might have one but idk how common that is.

[Geof]

... I'm under the (mistaken?) assumption that all hot rolled steel was soft, gummy and relatively easy to work with....

The first part of your assumption, hot rolled steel is soft and gummy, is correct; the second part is not correct.

Hot rolled mild steel, 1018 or something like that can be difficult to work with; especially when you have a machine with limited rigidity and horsepower.

Here is what I have learned from my experience:

Hot rolled machines best with negative rake tooling running fairly fast such as 400 or more fpm taking a decent cut per tooth and a decent depth of cut with a powerful airblast. This is how you remove material fast to get close to size or if your tolerances are loose to the finished size.

When you want to put fine detail or just take very light cuts off hot rolled then your tactics have to change and you drop the speed, feed per tooth and depth of cut, drown everything in coolant and probably use positive rake cutters. You definitely don't remove material fast.

For a novice working with hot rolled can be a PITA especially with a marginal machine whic to some extent is your situation.

Somewhere up the page someone suggested going to leaded steel and this is definitely a good idea. It is possible that you would be ahead even if you had to use leaded steel round bar and chew your shape out of that.

You embarked on trying to do this yourself because shops in the area wanted $800 to $2500. That is a wide spread: How many shops did you contact? Did you provide them with proper working drawings or CAD files? Were these quotes for one piece or the total cost for a couple of dozen pieces?

Right now it is my opinion you are in a hole and you don't get out of a hole by digging it deeper.

[handlewanker]

Hi Panz, first if you are using a 1/2" end mill to remove any significent amounts of material you're wasting your time and money.

I just sold my Bridgeport, (my mate wanted it), and I bought another mill, an Ajax with 54" table, slightly bigger, but with fast traverse and feeds in all directions and built in coolant pump.

I use a 2" HSS shell end mill running at 150 rpm to mill the outside faces and only go to smaller end mills or slot drills for slot or cavity work.

I also use a single point HSS fly cutter that sweeps a surface area of 2" to 3" wide, but in all cases You MUST use coolant, water based, otherwise you'll burn the tool point and that's expensive to get resharpened, especially end mills and slot drills.

3 in 1 oil is not to be used at all, except maybe for tapping smaller threads.

Fly cutters in HSS are the cheapest to use and easiest to resharpen, using only a bench grinder, if you know how.

I also had one of those three carbide insert end mills, but found that it was not cost effective for general machining, due to the inserts chipping easily, but very handy for machining cast iron.

The important thing also is to keep your body parts AWAY from ANY coolant especially allowing your hands to get soaked, otherwise dermatitus is a price you pay.

It is also a very wise precaution to use a barrier cream when doing anything in the metal trade, as there's so many nasties that can get into your skin, and at the same time if you aren't using eye protection all the time on the mill you're a masochist waiting for an accident to happen.

It doesn't take much coolant to keep the tool cutting, I used a plastic squeezy bottle for years, but a coolant pump system is more efficient.

Here again if you use a coolant pump you'll also need to have some sheet metal shields that keep the water from being sprayed everywhere.

Generally the hot rolled mild steel is cheapest and doesn't have the inbuilt stresses that cold rolled gets from the cold forming process, hence the name.

Once you've milled the outside faces of the hot rolled you'll have clean steel to work with, so just buy your material a bit oversize to start with.

The beautifull stuff is the S12L14 which is leaded mild steel, which has lead included in the mix to make the swarf come off in small chips.

Second to that is S1214 which is a freecutting mild steel, having sulphur added to the mix, also to cause the chips to break up, and is a bit cheaper than the leaded type.

In all cases you want to work with HSS tooling with positive rakes to the cutting edge, otherwise you'll be faced with a heap of chipped carbide tooling that is useless for anything.

HSS is the most user friendly cutting material, and can be worked using the average bench grinder.
Ian.

[panz]

Hey guys,

Thanks for the feedback. I've had some great success with 1/2" carbide 4 flute endmills. After removing the angle base on my vise I've managed to greatly increase the rigidity of the setup. Turns out the center post on my angle base is too high, causing the vise to be supported only by the 1" post and two 1/2" clamp bolts on the outside.

I tried going back to the 1604 APXT 3 insert mill, but I'm still having problems with the leading edge chipping. However, going the solid carbide route, I can pretty easily hog at 0.25" DOC, 0.5" wide, at 175 SFM and 3 IPM feed on uncoated carbide without coolant. I'm starting to look into a lube mister to maximize the endmill life - but I'm still on my first carbide endmill, so I'm not really sure what life I should expect out of the tool. I'm planning to pick up a TiALN coated carbide tool to see if I can get the SFM cranked-up a little higher.