PDA

View Full Version : Hundreds of Feet of Slot Cut Into Bottom of Aluminum Door Track



GEe
05-07-2018, 09:25 PM
Hello. We are working with aluminum track for heavy sliding glass doors.

A channel (approximately 1/2" square) runs the length of the track. Into this channel, a stainless steel extrusion is inserted to support the door wheels. In order for the s/s insert to interloc correctly with the aluminum track, we need to machine a slot into the bottom of each side of the channel.

These slots are about .125" tall and the depth of cut is only about 0.04" deep. The tolerance is not too demanding -- more in the order of 100th's of an inch than 1000th's.

The first challenge is this: we may have about 350 ft of track -- so upwards of 700 ft of slot to machine. And some of the individual lengths are about 30ft. The other challenge is that we are architects managing the construction of a home -- not machinists... So please forgive the following proposal:

Because the tolerance is relatively forgiving, we are considering guiding the track across a router or drill press with a keyseat cutter.

For example, this: http://www.harveytool.com/ToolTechInfo.aspx?ToolNumber=970395-C8

Is this conceivably possible?

Thanks very much! (It looks like I am not permitted to attach images or I could provide a drawing.)

George Bulliss
05-08-2018, 07:31 AM
Bumping this back to the top; got stuck in the moderation filter overnight.

Lew Hartswick
05-08-2018, 07:58 AM
A Router table MAYBE, definitely NOT a drill-press. The chuck on a drill press will not hold for that sort of side load and the shank of the cutter is going to be hardened so it will slip in the jaws.
good luck how ever you do it. :-)
...lew...

Magicniner
05-08-2018, 07:59 AM
Drill press spindle bearings are not designed for side loads, with some easily made guides for the work you could do this job with a 1 or 2 flute milling cutter in a router table.

Stepside
05-08-2018, 08:37 AM
Router table with a long fence and "feather boards before and after the cut as well as on top of the part. Also In-feed and out-feed supports. Do not "Climb Mill.

Baz
05-08-2018, 08:43 AM
A router is feasible with a guide assembly made with lots of ball bearings, some to guide it parallel, one each side to ensure the depth, and top and bottom to keep it at the bottom of the channel. During the cut you will be able to hear a change in note if anything moves and changes the position of the cutter.
Kerosene is a traditional lubricant for aluminium but with the motor underneath that is a problem. One of the problems with aluminium extrusion is that it is 'gummy' and sticks to the cutting tool.

SGW
05-08-2018, 08:46 AM
If the drill press chuck is mounted on a taper, the side loading will quite likely cause it to fall off. Inconvenient at best.

To Stepside's router suggestions, I might add something that he sort of implies, but doesn't state directly: cut one side at a time. If you're not familiar with the term "climb mill," it's when the work is fed so the rotation of the cutter tends to pull the work towards the cutter. Feed the work against the rotation of the cutter.

MattiJ
05-08-2018, 09:04 AM
Router with good guide assembly sounds workable to me. Or possibly even a circular saw!

MattiJ
05-08-2018, 09:07 AM
Drill press spindle bearings are not designed for side loads, with some easily made guides for the work you could do this job with a 1 or 2 flute milling cutter in a router table.

Typical cheapo drill press deep groove ball bearings handle side loads actually better than axial loading. But everything else is still unsuitable for milling.

Bellingahmster
05-08-2018, 09:38 AM
I can't quite picture the geometry, but if it'll fit, a table saw with a carbide blade would have that done in minutes. Same work hold-down (feather boards, bearings, etc.) as with a router table, but much higher feed rate. Lots more cutting edges in a 40T saw blade than a 2 flute router so heating and gumming up will be much reduced. Also no issue with climb milling - assuming you're feeding from the correct side of the table saw!

flylo
05-08-2018, 09:41 AM
I'd use a real wood shaper instead of a router.

lynnl
05-08-2018, 10:27 AM
Either I'm not understanding the issue, or most of the rest of you aren't.
The 1/2" sq channel is already there. He's now wanting to machine a .125" x .040" T-slot at the bottom of that channel.
There's no way a circular saw blade can be put into play here. A T-slot cutter is all I can think of.

If a milling machine is not available, either a router table or drill press sounds doable to me. .040" x .125" is not a lot of meat to remove; and there won't be much, if any, axial force tending to pull the cutter/arbor out of a drill press.

More concerning is the 30ft lengths. That's a long way to feed a piece!

boslab
05-08-2018, 10:46 AM
I don’t understand how you would achieve an undercut on a table saw, or wood shaper, a router could do it, the stainless is obviously inverted top hat, it would seem sensible that the track supplier also sells appropriate channel extrusion?
However if your determined that cutter would suffice or a keyhole slot cutter, lets going to be a challenge whatever you use, I’d be tempted to dress the lip off the track and epoxy it into the channel myself.
However welcome to the madhouse, sounds like you’ll be tight at home judging by your latest self imposed torturous quest,
Mark

cameron
05-08-2018, 10:47 AM
Deleted, misunderstood the problem, seems like I need to work on my reading comprehension.

Magicniner
05-08-2018, 11:05 AM
Read the OP again, it's not a T slot but it is 2 slots, one in either side at the bottom of the vertical side wall.
I'd grind relief on a carbide cutter designed for aluminium and do the job on a router table, one cut for each side.

old mart
05-08-2018, 11:29 AM
However the cut is produced, I would recommend a thin film of lubricant such as WD40 just on the area to be machined to keep the cutter from clogging up.

J Tiers
05-08-2018, 11:31 AM
Another kicker here is that the slots are almost certainly supposed to be all the way down on the floor of the groove. So the cutter needs to cut so that the two slots have their bottom face in line with the floor of the extruded groove.

A t-slot type cutter should do that, but a keyway cutter may not be as good at it. But keyway cutters are made in a suitable size (width). As long as the center is relieved, which it usually is, the cutter should work. The linked cutter is of the right type, and if it will reach into the extrusion it ought to be OK. I cannot tell if it is carbide or high speed steel.

I think the key to this working is going to be a good rigid guide that holds the extrusion position vs the cutter as the extrusion is slid past the cutter. You will need to guide it on all 4 sides.... The table and router setting will set the depth, and you need to have a hod down to prevent the extrusion from lifting, as well as left and right side guides to hold the cut depth reasonably well.

getting rid of the chips may be an issue also, you do not want them building up inside the groove of the extrusion.

At router speeds, a regular high speed steel cutter may not be good, even for aluminum, it may heat up and become dulled. A carbide cutter is more expensive, and a bit more fragile, but it will stand the high speed (rpm) better.

Your workmen should be able to handle the slotting job, if they are reasonably clever. maybe you are asking here because they are NOT so clever?

danlb
05-08-2018, 12:40 PM
Is it acceptable to have this .125 inch x .004 inch side groove for the entire length of the channel, or do you only want it a few inches long every X feet?

That will make a difference in the techniques that you will use. If every X feet you will want to make a jig with stops to position it and you will need a way to keep the cutter from hitting the track as you move it around.

Dan

Rustybolt
05-08-2018, 12:58 PM
Use a table saw with a dado blade. Much easier to control depth and width of cut.

oxford
05-08-2018, 01:42 PM
A picture of the track you are working with will help determine a way to deal with the problem.

GEe
05-08-2018, 02:30 PM
This has been extremely helpful -- thanks everyone very much for the feedback. We'll see what happens....

J Tiers
05-08-2018, 03:26 PM
Folks... what he has is the one o the left, what he wants is like the one on the right

https://i.imgur.com/sKIY0a1.jpg

There will be other stuff around it , but that's the basics of it, as he explained the matter.

Saws will NOT get down in there. only something like a t-slot or woodruff key cutter will do it easily.

GEe
05-08-2018, 04:08 PM
Thanks J Tiers -- that is indeed the essence of the geometry.

Since it sounds like a keyseat cutter in a router could do this, I have two related questions (but someone please let me know if these should be in separate threads):

1. The existing track is already anodized. I'm not concerned about the visibility because it is at the bottom of the track, but presumably corrosion at the cuts could be a problem. Is there a thin, permanent sealer of some kind that could work in a case like this?

2. As others have noted, the length of cut is concerning. Any guess how many feet we can go before overheating or using up the cutter?

Thanks again everyone.

PStechPaul
05-08-2018, 05:31 PM
If the channel is hard anodized, it might cause pretty rapid wear on a cutter, so carbide might be necessary.

Another idea might be to make a broach that could form the slot from each end, as long as the slot does not need to be very long. It is only necessary to take 40 mils which might be done with four steps of 10 mils each. I found some 1/8" x 1/8" broaches that might work. You could use two of them with a spacer in between to enable cutting.

https://cdn.mscdirect.com/global/images/ProductImages/0030024-23.jpg

https://www.mscdirect.com/product/details/00300244

J Tiers
05-08-2018, 05:39 PM
A carbide cutter will do that all day, I'd expect one to last the whole job, although if something goes wrong, that could be different. Going wrong can be feeding material too fast, chipping the cutter when starting on a new piece, that sort of thing. Might be wise to have at least one extra if you go that way.

I cannot predict how long an HSS (High Speed Steel) cutter will last. The routers usually are high RPM, somewhere perhaps 10,000 rpm I think? If the cutter is 3/8" diameter, then it will be almost 1 1/4" circumference. At 10.000 RPM, that is 12,500 inches per minute, or about 1000 feet per minute. that is certainly at the high end of the range even for cutting aluminum, and if the feed is not kept up, the tool may "rub" instead of cutting, which tends to dull it.

I'd expect HSS to dull pretty fast at that RPM, if allowed to rub. Once dull it will heat up and not cut well, and it will get duller and duller. You will notice it being harder to feed material through, and that is a signal to change cutters.

It may be cheaper to use HSS and have more extras.

You can also slow the router down to where an HSS cutter is less likely to be "burned up" (dulled by rubbing and overheating).

danlb
05-08-2018, 06:54 PM
The broach may be a good idea, but a router and carbide bit are easier.

I'll do the math for a specific sized cutter when I come back from doing some chores. That will give you a valid (not optimal) RPM, size and maybe even a part number! :)


Dan

Magicniner
05-08-2018, 07:01 PM
The broach may be a good idea


we may have about 350 ft of track -- so upwards of 700 ft of slot to machine. And some of the individual lengths are about 30ft

Hmm, I wouldn't fancy broaching that :D

garyhlucas
05-08-2018, 07:07 PM
Do they make the track you need? Because I get that this is an expensive problem but I see this as getting a whole more expensive. I have a reputation for doing stuff like this. However I would definitely give this a pass.

Boostinjdm
05-08-2018, 07:18 PM
In this thread we learn who speaks before understanding what they read. Or didn't read.

I have done similar in a t slot track. I used a router and a homemade keyseat style cutter with a guide bearing on the shank. Yours could be done better with a router table, fence, and feather boards.

GEe
05-08-2018, 08:05 PM
The broach may be a good idea, but a router and carbide bit are easier.

I'll do the math for a specific sized cutter when I come back from doing some chores. That will give you a valid (not optimal) RPM, size and maybe even a part number! :)


Dan

Thanks, Dan. I did end up ordering the Harvey Tool I linked to above (part 970395-C8). Of course, let me know if I went the wrong way with that...

danlb
05-08-2018, 08:55 PM
I'm going to give the "how it's made" version so that you can figure out for yourself what cutters and speeds will work. Some of the numbers used are derived from the chart provided on the web page you bought the cutter from (http://www.harveytool.com/FileCheck.aspx_Q_ToolNumber_E_970395-C8_A_FilePathName_E_SpeedsFeeds%7cSF_962900.pdf). Fortunately, you can go slower in aluminum without causing problems. I'm assuming that you are going up one side and then down the other.

First we get the RPM. The RPM is derived from the tool size, the material being cut and the tool design. Assuming that it's one of the common alluminum alloys, I'm guessing that 700 SFM will be close enough. That number is used in the calculation for RPM. The cutter you chose is 1/4 inch diameter. It's HSS (hard steel) with a titanium dioxide coating that aluminum does not stick to very well. The cutter is 4 tooth.

RPM = SFM / (.2618 * cutter diameter in inches)

Solving gives us
RPM = 700 / (.2618 * .25)

RPM = 700 / .0654

RPM = 10703

The data sheet from that supplier says that the chip load is .00136 inches per tooth. You have a 4 flute cutter, and you are only taking .004 deep so that should work OK when pushed through at a moderate speed.

Something to consider; If you are using an upside down router on a router table you will have to take steps to ensure that the aluminum shavings don't shor out the motor. You will want to avoid climb milling, as mentioned already.

Hope that helps.

Dan

Robin R
05-08-2018, 09:20 PM
If you can send the bit back then this might work, it even has a bearing to limit the depth of cut to 0.062". http://www.leevalley.com/en/Wood/page.aspx?p=65641&cat=46168,69435,46176&ap=1 To guide the material over the bit, route a slot the size of the extrusion in a large enough piece of wood and clamp the whole assembly down to the router table. Once you have the position dialled in in relation to the cutter, you can just feed the work through in a relatively safe way.

RichR
05-08-2018, 09:40 PM
... The data sheet from that supplier says that the chip load is .00136 inches per tooth. You have a 4 flute cutter, and you are only taking .004 deep so that should work OK when pushed through at a moderate speed. ...

I thought he said the cut was to be 0.040" deep.

danlb
05-08-2018, 10:18 PM
Good catch Rich. I saw 2 leading zeros and thought thousandths. Robin has a better recommendation anyway. :) ( post 32 )

GEe
05-08-2018, 11:06 PM
First off -- thanks again for all of the help. Much appreciated!


Good catch Rich. I saw 2 leading zeros and thought thousandths. Robin has a better recommendation anyway. :) ( post 32 )

True about the .04". Does that significantly change my chance at success?


If you can send the bit back then this might work, it even has a bearing to limit the depth of cut to 0.062". http://www.leevalley.com/en/Wood/page.aspx?p=65641&cat=46168,69435,46176&ap=1 To guide the material over the bit, route a slot the size of the extrusion in a large enough piece of wood and clamp the whole assembly down to the router table. Once you have the position dialled in in relation to the cutter, you can just feed the work through in a relatively safe way.

Very interesting find. I think I can't make this particular bit work because the slot is actually just under 1/2" (.44") and so this particular bearing would not fit. But I'm not sure I understand the benefit since everything would be locked in between the table and the guide you described. Is the purpose of the bearing to better stabilizes the shank?

DR
05-08-2018, 11:12 PM
Is the track hard anodized? If so, even carbide may not last for all 350 feet.

Robin R
05-09-2018, 12:00 AM
The bearing on the bit was just incidental, here is one that is only 0.375" diameter. http://www.leevalley.com/en/Wood/page.aspx?p=30113&cat=46168,69435,46176&ap=1

J Tiers
05-09-2018, 12:20 AM
First off -- thanks again for all of the help. Much appreciated!



True about the .04". Does that significantly change my chance at success?



Very interesting find. I think I can't make this particular bit work because the slot is actually just under 1/2" (.44") and so this particular bearing would not fit. But I'm not sure I understand the benefit since everything would be locked in between the table and the guide you described. Is the purpose of the bearing to better stabilizes the shank?

The bearing also controls the depth of the cut...by how much the cutting edge sticks out beyond the bearing. Obviously the bearing stops the cutter from going deeper into the side wall. It does not, however, stop the cut from being shallower.

The 0,04" depth is actually better than a shallower one, because if the extrusion is anodized, the deep cut will cut well under the anodizing, and avoid having the cutter cutting it, for 'conventional milling" type cuts, where the cutter is pushing back against the material as it is being fed in. The cutter will cut plain aluminum, and come up under the anodizing, which will probably break away without having to be actually cut by the tool. Anodized aluminum is pretty much the same stuff as is in the wheel of a tool grinder. Highly abrasive.

If chips are not controlled, then the cut chips may be "re-cut" if they build up in the way of the cutter. That re-cutting can dull the cutter, or jam and break it. Blowing compressed air through from the side the finished extrusion comes out of can help clear chips, if air can get through. Blowing air from the router up and out past the cutter would maybe be better. Either one will also make a mess, and put the person feeding in the work in the way of the chips being blown out. But you need to get them out or there will be a problem in that little space inside the extrusion.

If the aluminum is anodized, carbide may be better, although, as I mentioned, HSS will work, and is cheaper when you break a cutter. Those cutters are not the toughest things in the world, and can be damaged by forcing the cut.

PStechPaul
05-09-2018, 12:43 AM
A rotary burr might do the job. I found one of the right size:

https://www.mcmaster.com/#4241a53/=1crem2g

https://images1.mcmaster.com/mvA/contents/gfx/large/4241a53p1l.png?ver=1265294202

NiftyNev
05-09-2018, 04:46 AM
Have you considered some sort of double sided adhesive tape?

ikdor
05-09-2018, 06:13 AM
I would look at modifying stainless insert and use 3M double sided tape to install it.
Depending on money involved and price of failure it might be worth it to investigate the cost of a custom extrusion. Then you have a perfect product.