[tmarks11]

I don't see why I can't do the same thing with 36" inch sections on the smaller machines.

If you look at the Novakon Torus Pro, I suspect that you will find it is not really much smaller than you knee mill with a table of 40x12".

?????? I'm not casting anything. I'm machining a 4 inch wide and 120 inch long profile INTO steel or aluminum.

The confusion comes from your calling this a steel mold. Generally you pour something into the mold and cast it. Most people assume that a mold is a one-off creation, and a majority of the production work is done with casting the product. It sounds in your case that machining the extrusion IS all of the production work.

Is this a one time production, or do you foresee making a lot of these? If you are making these over and over, than you should probably think seriously about the Haas TM2, since the increased horsepower and increased X-travel will help over time. Used TM2s sell for about $22-24k for mid-2000's models (without tool changer).

One real advantage to doing these on a open bed mill (like the Haas TM2 or Torus Pro or Tormach) instead of your existing knee mill is that you could set it up with roller tables on both side, and machine the entire 10' section in one go, with just sliding it and re-clamping it on the table as you finished machining each 18-24-40" section (depending on what machine you ended up with). A well built jig would be needed to make sure you keep alignment between cutting sections.

As long as we are pouring time and money down a rabbit hole: cnc X-Y table with 15k spindle mounted on a moving gantry that can cut the extrusion all in one setup. Make the table 12" wide and 10' long, and it should be plenty rigid enough for machining aluminum. Down-side: can only make one type of thing.

[Steve Seebold]

Why not make your molds from 7075 instead of 6061?

Yes, a Tormach PCNC 1100 will make your molds. As will a Haas.

I have owned a PCNC 1100 since July 2011, and I am the former owner of a Haas TM1 and a FADAL 3016 box way machine and a Tormach will do anything those machines will do, it's just going to take about 3 times longer.

I run some of the same jobs on my Tormach that I ran on those machines, and outside of a profiled hole being about .001 out of round, everything else is perfect. I have run several jobs that requires +/-.001 on a slot width, and I was able to hold that ALL DAY LONG.

I read a lot about people having their Tormach making errant moves, but I wonder what CAM software they are using. I program my machine with GibbsCam, and I have never had it take off and do its own thing.

Another thing I have done is, I have switched to a Quad 1 vise which has the fixed jaw on the front of the vise. That way, I am constantly working in a X PLUS Y PLUS direction. If your fixed jaw is on the back of the vise and you pick up on the back left corner of your part, you will be working in the X PLUS Y MINUS direction. I think what might be happening with the folks whose machines are making errant moves is when they make a Y axis edit and the move they are editing is a Y MINUS move, when they make the edit, they forget to add the MINUS sign and then the machine moves in the PLUS direction, destroying their part.

[Spartan1]

As Ray said, buying a machine to do these yourself is by far the most expensive option.
You can get your mold made for $3000, and start making money with it,
or,
You can pay $20K, spend a few hundred hours learning how to use it, and then another 100 hours to make your mold.

Get the mold made, make your money, and buy a hobby machine when you retire.

The economics don't work out that way.

Machining one mould is $2,400 and makes ONE product per cycle. I can only get a limited amount of cycles an hour. To the operator, there is very little difference if he makes one product at a cycle or 5 products a cycle. To me, as the owner, the difference is.......1 product per cycle is okay for start up but I'm playing around versus 5 products per cycle and it's a profitable business. So invariably, I need to make 5 identical moulds per product. Then multiply that by the amount of different products.

The start up with 5 different products and their individual moulds is $12,000. Multiply THAT by 5 or $60,000 to get into serious production. (NO, I can not make 5 different products per cycle unless I want to guarantee a mistake and damage the moulds). Every subsequent product will need it's own set of moulds.

The short term is one thing, the future means I MUST buy a CNC.

[Spartan1]

Why not make your molds from 7075 instead of 6061?

It's expensive and ultimately, 316ss or 4130 is much tougher. I don't really want to go with aluminum but the upside is that it's easier to machine with smaller equipment. And also easier to polish.

[Spartan1]

The confusion comes from your calling this a steel mold. Generally you pour something into the mold and cast it. Most people assume that a mold is a one-off creation, and a majority of the production work is done with casting the product. It sounds in your case that machining the extrusion IS all of the production work.

ONE mould will makes ONE specific product at time multiplied by many cycles . In the case of hardened and chromed 4130, Short of an accidental damage, it should make hundreds of thousand...if not a million cycles.

The catch is...the moulds cost is completely irrelevant in a mature product range....but a new product range AND the amount of moulds makes it the "what do I do" head scratcher.

[Spartan1]

Again and again....I like to thank those who participated in this thread. You opinions and ideas are helpful to draw a conclusion.

So far.....some conclusions

*The small machines will do the job in all of the material but it will take three times longer.

*It's going to take time to learn the machine.

*Small machines are not THAT cheap and they start to push into the range of the cheaper of the simple larger machines (TM1 and TM2).

And last but not least conclusion.....I should retire and go fishing! LOL!


(And I'm going to talk to Tormach/Novakon tomorrow plust try to arrange a visit to a TM1/2 owner.)

[BAMCNC.COM]

When people say something takes longer on a Tormach - that isn't always the case. Take my parts for instance, they are all Grade 5 Titanium - you are pretty much stuck under 200SFM, and that goes for any mill. So the only time I would save is when the endmill isn't actually cutting. Depends on how you design/code things aswell. I base all of my stuff off of 1 tool if possible. Of course Aluminum.. yes.. the More HP and the faster the rapids, the faster you can cut - it's almost unlimited.

I suggest checking some material SFM charts to be a leading decider in what you actually need for a machine. If I had to go back, I would probably get a Tormach 770 as when doing 1/16" endmill or engraving I could use the extra spindle speed.

[Hirudin]

To make that... object... you can reduce your tooling budget considerably. No need for vises as you can just bolt it directly to the table or a sub-plate. You could get two of them onto the PCNC 1100 table or three onto the Torus Pro table. Rough the entire thing with a 1/2" end mill and pre-finish with a 1/2" ball mill. Maybe jump up to 3/4". Other than that you'd probably want a dial test indicator with some kind of magnetic base. No need for an ATC, power draw bar, or any other conveniences. I'd just put the tools right into an R8 collet and set the Z with a gauge block (add that to your shopping list). Oh, you'll want an edge finder too - get one with the same size shank as the tools you plan to use. Should run you a few hundred dollars in total.

CAD and CAM shouldn't cost you very much either with a shape like that. The pre-finish operations wouldn't be any more than a series of straight lines.

How long will it take? Stab in the dark: maybe six hours per section of object. Start in the morning, change the tool in the afternoon, bingo bango.

I still think it's impractical, but to make the object, as described, you could probably be on your way for $12,000 or so (ignoring the learning curve and Murphy's law).

[Steve Seebold]

First of all, my drawing is misleading. Its' a lot more complex then the the opening post. See below.

The shops I have gone into are telling me that they have to use a 1/2 ball bit and run it in .015" step increments. After that, to make it smooth, I still have to either sand it in the case of aluminum or grind it in the steels. They are quoting upwards of 20 hours at $120 in a 10 foot CNC....and they tell me that's dirt cheap.

I can NOT design the mold to suit the CNC and end mills, I have to design an attractive product and then blow my money/mind on machining the mould.

With my knee mill, I had a custom made carbide head ($700) that had the entire 4" profile and ran it on aluminum. Of course, I was sweating bullets hoping it didn't crack the carbide. I was told a profile cutter to handle stainless would make me cry. Plus, I have zero ability to change the design.

Yes, in the future, I can buy a Haas, but right now, our sales are peanuts and $40K will hurt a bit. Plus there is no real need for it because we are NOT a machining company, we are in a completely different field. If we don't need moulds, the machine will sit idle.

I am NOT a machinist, I am an engineer that is competent around machines so I have to "dig" to get all the information. I'm hoping/praying/wishing that I can do this in house in order to have the flexibility and also be able to make smaller runs without massive costs for each mould.

THANK YOU to all who participated. I am grateful for any info and direction!

The mould face is 4" wide, 2" high and runs 120"...in sections......

Attachment 245748

That's an easy part to do on a Tormach. Time consuming, but easy. I would do the heavy hogging with a 3/4 inch 2 or 3 flute insert end mill and finish the radii and the corners with something smaller. Yes, insert tooling is more expensive than solid carbide, but the straight flutes all but eliminate the cutter wanting to pull down during heavy cutting. I would probably make a program that takes most of the material out by plunge ruffing.

I would make them in 15 inch sections so you're not working against the limits of the machine.

The first thing I would do is screw and dowel the sections together on both sides, then number each section so you get them back in the same place after you're finished machining.

I would also look for an aluminum supplier who could provide you with finished blanks that are all the same size and square on the ends. You'll pay a little bit more for your material, but you won't have to be concerned about material consistency.

I don't have the ATC on my machine, but I do have the PDB. The ATC wasn't available when I bought my machine. It came about 3 months later.

The ATC would be nice for the job I'm running right now. This part takes 27 minutes and requires 9 tools. One of which runs for 13 minutes.

That's OK this time because while this part runs, I am packing boxes. I'm moving my machine to a new location in about 10 days.

Most of my jobs require 1 to 3 tools, and run fast so I have to stay right at the machine anyway.

[SCzEngrgGroup]

Machining one mould is $2,400 and makes ONE product per cycle.

And for that same $2400 you could probably get several, perhaps 5 or more, molds using extrusions, with $0 capital expenditure, and zero learning curve....

Regards,
Ray L.

[Spartan1]

Steve and Hirundin, thank you. This the kind of information I'm trying to get.

Steve, (or anyone)......any chance you can give me a ballpark on time with the following criteria.....

1...Assume that all the moulds will need to finish with incremental passes of .015" steps with a .5 inch carbide ball mill. In other words 260 passes to cover the 4 inches width by the 16 inch legnth.

Hogging....I'm removing I.5 cubic inch of material per lineal inch with a roughing mill. Or about 180 cubic inches per 120" mould. Or 24 cubic inches per 16". Probably no more then a dozen passes. I don't think that is major time unless you tell me otherwise.

2.....in 6061 aluminum.....mild steel....4130....316ss.

What is your best guess per 16" legnth? Your answer is half the decision.

[tmarks11]

CAD and CAM shouldn't cost you very much either with a shape like that. The pre-finish operations wouldn't be any more than a series of straight lines.

No need for CAD or CAM for the profile he showed. Simple trig and the g-code for that should only take a matter of minutes to code. You could hire a student from the local vo-tech college to write it for you if you don't want to learn it. The classes I took, students were writing much more complicated code in the middle of their first CNC semester.

That's OK this time because while this part runs, I am packing boxes. I'm moving my machine to a new location in about 10 days.

Steve, let's co-opt this thread too and talk about moving.

...you could probably get several... using extrusions, with $0 capital expenditure, and zero learning curve....

Although it really sounds like he should be making these out of steel instead of aluminum. Using them to stamp an impression in something?

[David Bord]

Spartan,

Do you WANT to learn to CNC machine? If thinking about playing with one in retirement, my guess is... If yes, just do it... I knew nothing about it before buying my Tormach. I bought basic and upgraded over time... I have to say its one of the best purchases I've made in my life. It's been challenging to learn having basically no machining experience(manual as well) but have never regretted it.

Tormach has customer service that is second to none, they are truly outstanding.... and that is important when getting started.

Keep in mind, the Tormach is based on an open standard, so is inexpensive to repair if it's ever needed. The same cannot be said for larger mills. Also, Tormach has proven to have a pretty good resale, which means you can sell it and only be out a few bucks IF it didn't work out.

Check the price for tooling on larger mills as well(holders etc). My guess is they are significantly more expensive. Bigger machines are fast... Means things can got to heck pretty fast as well.

Whatever you do, good luck and keep us posted on your decision.

David

[Spartan1]

Spartan,

Do you WANT to learn to CNC machine? If thinking about playing with one in retirement, my guess is... If yes, just do it... I knew nothing about it before buying my Tormach. I bought basic and upgraded over time... I have to say its one of the best purchases I've made in my life. It's been challenging to learn having basically no machining experience(manual as well) but have never regretted it.

Tormach has customer service that is second to none, they are truly outstanding.... and that is important when getting started.

Keep in mind, the Tormach is based on an open standard, so is inexpensive to repair if it's ever needed. The same cannot be said for larger mills. Also, Tormach has proven to have a pretty good resale, which means you can sell it and only be out a few bucks IF it didn't work out.

Check the price for tooling on larger mills as well(holders etc). My guess is they are significantly more expensive. Bigger machines are fast... Means things can got to heck pretty fast as well.

Whatever you do, good luck and keep us posted on your decision.

David

Of course I want to keep it. How else do I torment the big boss by trekking filings around the house! LOL!

It has to earn it's keep first......and then she can bury it with me.....

[Steve Seebold]

Steve and Hirundin, thank you. This the kind of information I'm trying to get.

Steve, (or anyone)......any chance you can give me a ballpark on time with the following criteria.....

1...Assume that all the moulds will need to finish with incremental passes of .015" steps with a .5 inch carbide ball mill. In other words 260 passes to cover the 4 inches width by the 16 inch legnth.

Hogging....I'm removing I.5 cubic inch of material per lineal inch with a roughing mill. Or about 180 cubic inches per 120" mould. Or 24 cubic inches per 16". Probably no more then a dozen passes. I don't think that is major time unless you tell me otherwise.

2.....in 6061 aluminum.....mild steel....4130....316ss.

What is your best guess per 16" legnth? Your answer is half the decision.

If you can send me a drawing of the end configuration I'll run it through my cam system and I can hit the run time pretty close. Are you planning to use carbide or HSS cutters?

BTW, 16 inch sections takes 7.5 pieces. 15 inch sections takes 8 pieces.

Email drawing to [email protected]

You can send it as .dxf, or .igs

[Spartan1]

If you can send me a drawing of the end configuration I'll run it through my cam system and I can hit the run time pretty close. Are you planning to use carbide or HSS cutters?

Send it.

Depending on the times/info you send back, I may go into it full steam.....or locate a cheaper CNC shop.....or give up fighting China Inc and go fishing.

BTW....all my end mills are carbide or insert cutters.

[Hirudin]

[edit]Oops, I didn't see Steve Seebold's offer above. Looks like you'll have two estimates. [/edit]

I guess I got curious so I CAMmed a similar shape to see approximately how long it might take to mill a 15" section of a similar shape out of 4130. What I did was rough most of it with a 3/8" end mill and two slotting passes with a 1/2" ball mill. For finishing I had it use the 1/2" ball mill with a 3D step-over of 0.381 mm (0.015").

Note: I have cut very little steel, these numbers are from G-Wizard primarily. I also rarely slot, so I don't know if these numbers are anywhere near what would be possible or optimal in reality. The time estimates employ rapids of ~400 IPM.

Roughing parameters...
3/8" 4-flute carbide end mill
Feed: 397.5 mmPM
Speed: 2312 RPM
DOC: 2 mm
Stepover: 65% (first pass of every level is a slot)
Estimated time: 1:03:35

1/2" 4-flute carbide ball mill
Feed: 331.7 mmPM
Speed: 1867 RPM
DOC: ~4 mm
Slotting cut
Estimated time: 0:02:31

Finish parameters...
1/2" 4-flute carbide ball mill
Feed: 700.2 mmPM
Speed: 1888 RPM
Stepover: 0.381 mm
Estimated time: 03:27:37

[Spartan1]

[edit]Oops, I didn't see Steve Seebold's offer above. Looks like you'll have two estimates. [/edit]

I guess I got curious so I CAMmed a similar shape to see approximately how long it might take to mill a 15" section of a similar shape out of 4130. What I did was rough most of it with a 3/8" end mill and two slotting passes with a 1/2" ball mill. For finishing I had it use the 1/2" ball mill with a 3D step-over of 0.381 mm (0.015").

Note: I have cut very little steel, these numbers are from G-Wizard primarily. I also rarely slot, so I don't know if these numbers are anywhere near what would be possible or optimal in reality. The time estimates employ rapids of ~400 IPM.

Roughing parameters...
3/8" 4-flute carbide end mill
Feed: 397.5 mmPM
Speed: 2312 RPM
DOC: 2 mm
Stepover: 65% (first pass of every level is a slot)
Estimated time: 1:03:35

1/2" 4-flute carbide ball mill
Feed: 331.7 mmPM
Speed: 1867 RPM
DOC: ~4 mm
Slotting cut
Estimated time: 0:02:31

Finish parameters...
1/2" 4-flute carbide ball mill
Feed: 700.2 mmPM
Speed: 1888 RPM
Stepover: 0.381 mm
Estimated time: 03:27:37

I'm really surprised at the roughing times. My totally amateur guess would be 30 minutes or less with a half inch carbide roughing mill.

4.5 hours a 15 inch section roughly corresponds to 80% more then the 20 hours of a monster Haas doing it in one go.

Is 316ss roughly the same time?

NOBODY in my plant makes $2,400 a week. I can set up the tooling and mount three moulds at a time while my operator change tools and baby sit it. I'm at $700 per mold. 10 moulds and the machine is free.

I'm not crazy....and 4130 thank you's!

[clockwise]

What machine are these long moulds going into? A press? Or is this moulding composite products?

[Hirudin]

My numbers could be way off. I went with the 3/8" bit to get into the bottom rounds a little, but then I ended up slotting with a 1/2" ball mill anyway, so maybe I should have used 1/2" square mill after-all.

I usually do my roughing with torchoidal tool paths generated by SolidCAM, I wanted to get an idea of what kind of times simpler tool paths would produce. This is actually faster than the torchoid-based settings I tried.