[motoeng]

A little background info first. Currently I have an outside supplier manufacture this item (and several others with similar geometry). They do an excellent job at a reasonable price - absolutely no complaints.

However, since my orders are what I assume to be relatively small dollar amounts in comparison to their other jobs, my lead time is usually 7-8 weeks and I must order at least 500 pieces at a time to bring the piece price into a range I find acceptable. Considering it takes me a while to sell those 500 pieces, this process ties up $$ that I'd like to use to manufacture other parts.

Additionally, I'd like to be able to create new designs in small batches (let's say 5-10 pieces) and see how they sell before committing myself to a production run. The piece price to have a shop make that number of parts is just not economical.

Hence my desire to try and bring at least some manufacturing capabilities in house. As far as my technical background is concerned, I am a mechanical/civil engineer by day and have good experience designing machined parts in SolidWorks. I've been doing my home business for about 5 years and have built up a decent customer base for my products. I've recently started learning Fusion 360, and was able to create this part in F360 after a couple hrs of learning the interface. However, when it comes to actual machining and CAM, I have ZERO experience.

So, I realize I'm looking at a steep learning curve to go from CAD to actually being able to make these parts on a CNC machine, Tormach or otherwise. But the wealth of knowledge here and strong community behind the Tormach product lines makes me think it just may be possible for me to teach myself how to machine some of my parts myself.

That said - while I've lurked here, I don't really know if I could make the pictured part on a Tormach at a similar quality as I'm getting from a professional machine shop. I think with a well equipped 770 or 1100, with a Rapid Turn, broaching tool, and the right end mills it may be possible. But would it require such a long time to make each piece, that it wouldn't be worth the hassle? Better to just leave it to the professionals?

The part is 6061-T6. Threads are M20x2.5, and the height and largest outer dia are both around 29 MM.

In a nutshell, I think have an idea of how this part is made in real life:

1. Turn the overall outer profile
2. Cut the threads
3. Drill/bore the bottom hole
4. Cut off part
5. Switch to the vertical milling ops.

Besides the two small through holes in the sides of the part, I would think the vertical milling can all be accomplished in one setup in 2D. I'm not sure how some of the angled chamfers would be accomplished though, unless I can order chamfering cutters with the correct angles? The small through holes I'm assuming would have to be accomplished with either some creative fixturing, using the indexing feature of the Rapid Turn, or a 4th axis setup.

Your thoughts would be appreciated!

[coffeetek]

Welcome to forums.7-8 weeks lead-time on larger quantities is pretty normal in my experience. You might sometimes get lucky and it ends up being less but that's about normal.I am far from being an expert machinist, but I know a little bit... Lot of stuff going on that part. I do not have experience with RapidTurn, but I think that is a light weight solution. Tormach Slant Pro will do turning for that part easy and to excellent tolerances. You can then mill it on 770. Now to the cost of 770 alone... I doubt you can justify buying it if you do the math. If you take what you are paying to machine shop to make that part, how long it will take you to pay off 770? Add to that anytime you'd pay them extra to make you low quantity 5-10 pieces... I think you might find that it takes a heck of a long time to pay machine off. Don't forget that machine is just small part of the cost, large chunk on top of that goes for tooling.Then it will take you some time, months likely, to learn how to machine and work-hold just that one piece...I am not trying to discourage you just giving you something to think about in terms of the actual cost of making this yourself. Now if you want to make it for fun of it, then all this goes out of window, just get the machines and start making :-) Hope this helps.

[SCzEngrgGroup]

The Tormach is quite capable of making that part, but.... If you have no CAM/CNC experience, get ready for a steep learning curve. It takes years of hands-on experience to become really proficient. That's not a particularly complex part, but there are still a lot of tricks to getting something like that to come out to-spec consistently, in a time-efficient manner.

And I would have to question whether it makes financial sense to make them yourself. The commercial machine your current vendor probably uses to make those parts can turn them out 5-10X faster than a Tormach will. And with proper fixturing (another STEEP learning curve), they can make many parts in a single run, with little operator intervention. Doing the same job on a Tormach will most likely require a lot more "baby-sitting". So, it comes down to a trade-off of $ vs hours of your time.

What are you currently paying? What are the approx. dimensions of the part (OD and height are enough)?

Regards,
Ray L.

[motoeng]

Thx for the reply coffeetek, it is appreciated! I would love to be able to afford both a full size lathe and mill, but that's just not in the cards at this point in time. The release of the rapid turn got me thinking you could actually make a go of manufacturing parts that require both turning and milling, without having to invest in both a lathe and mill. From what I've seen in videos here and elsewhere, the turning required on this part could easily be handled by the rapid turn, but I've yet to see a video where decent sized threads are cut, so that would be a concern.

The tolerances on this part are very generous, +-.005 on most everything except for the threads and hexagonal hole which are controlled by their respective standards. Surface finish requirement is 32 Ra. As far as saving $$ by bringing manufacturing in house and being able to pay off the machine, you're right. It would take many years to accomplish that. Fortunately, I'm not looking at this avenue so much to save on manufacturing costs. Heck, I value my time considerably, so this route would actually cost me a lot more than paying someone else to do it. I'm more so looking at this as a way to add some flexibility to my business. My threshold right now as far as what I'm looking to spend would be around $15K - $20K. From what I can tell that would get me a base machine (770 or 1100) with deluxe stand, PDB, Path Pilot, Rapid Turn, and maybe some other goodies, and still have some left over for tooling. I think the ATC would be out of my price range.

[motoeng]

Thx Ray - no doubt my supplier can crank these out faster than I could ever dream of making them. During my busy season, I would need around 50 of these a week. I'm sure they are using a multiple fixture setup to reduce operator intervention. Thinking about it all makes my head spin. While I'd prefer not to reveal my costs for this part, it is very reasonable given it is manufactured in the US and the quality is what I consider to be excellent. Lets just say I pay well under $10/piece. I compete against Chinese sellers of similar products, and US sellers who manufacture in China, so I am definitely price conscious. While my parts aren't the cheapest in the market, my customers seem to appreciate the quality and customer service, so I'm thankful for that.

Let me be clear that I have no misconceptions about buying a machine and being able to rip out great looking parts consistently from the get-go. Knowing me, it would likely take several years to start to feel comfortable with the process. That said, it's obvious I don't plan on taking any work away from my supplier anytime soon.

[SCzEngrgGroup]

Here's how I see it:

If the ATC is out of your price range, then you should assume you will be pretty much baby-sitting the machine full-time when it's running, which means a lot of time.

The hex hole, BTW, can only be done using a rotary broach. But, that, and all the other "turned"" surfaces can be done on a mill, with no need for a RapidTurn. Think of using the mill as basically a vertical lathe, with the part mounted in the spindle, and the tool mounted to the table.

The threads can be cut on the mill using thread-milling.

Looks to me like you'd require at least 4 fixtures:
1) For turning OD, with the part in the spindle, and the tools mounted on the table
2) For milling the flats and broaching the hex, with the part mounted to the table with a fixture
3) For cutting the threads, with the part mounted to the table with another fixture
4) For drilling small holes, with the part mounted to the table with yet another fixture

You'd need several tools:
1) At least one lathe tool
2) At least one square end mill, for cutting the flats
3) A tapered end mill for cutting the angled faces between the flats. This assumes that is a rational angle, for which a tapered end mill is available. If not, this part gets a lot harder, and a LOT more time-consuming
4) A hex rotary broach and holder
5) Two drill drill bits
6) At least one chamfer tool, perhaps two
7) A threadmill

Without an ATC, toolchanges alone will take you 3-4 minutes per part, if making them one at a time. Machining time is probably another 5 minutes per part. The part will have to be re-oriented/re-mounted 3-4 times to do all the operations. So you could be looking at as little as 5 parts per hour. To improve that, you'd need to build mulli-part fixtures, optimized for maximum throughput, minimum toolchanges. Those fixtures will take time to develop and debug. Your very, very best throughput would still be limited by the raw machining time, which, at 5 minutes/part, means you'd never do better than 12 parts/hour. Again, without an ATC, you'll be largely sitting waiting to make a toolchange. Making 100 parts, if you REALLY optimize everything will take an absolute minimum of probably 10-12 hours. In reality, you'd probably be hard-pressed to do it in twice that time.

Regards,
Ray L.

[motoeng]

I certainly appreciate the dose of reality Ray! It's info like this that makes me love to read this forum.

I have seen some spindle turning before courtesy of keen's videos, but I wasn't entirely sure how it holds up to horizontal turning in terms of surface finish. Thread milling seems to me like it would take much longer than turning and the surface finish would not be as smooth, but this is just conjecture.

From what I'm understanding, the reality is that it will take some ingenuity in the setup/fixturing department to get this part made in a reasonable amount of time, even with an ATC. It makes me appreciate my supplier even more.

[Jim Dawson]

I'm going to disagree with Ray a bit. You can ''turn'' that part without putting in the spindle. You can circular interpolate the OD.

First do the top features, then flip the part over into the fixture in the soft vice jaws. Circular interpolate the thread major diameter, pocket hole, and mill threads.

Tapered endmills and chamfer tools are very available, and I also had a special built for $50.

So, the steps, all done in a 3 axis CNC mill. A tool changer would be nice, would save a lot of handling. Rather than just one part at a time you could fixture two parts in a vice.

1. Cut blank with a saw. rinse repeat for 50 parts. Or just buy them cut to rough length.
2. Drop into the vice soft jaw fixture
3. Face top
4. Mill outside profile
5. Pocket hole for hex
6. Change tool
7. Mill chamfers
8. Change tool
9. Broach hex
10. Done with the first side. rinse repeat for 50 parts.

Second side

1. Drop into vice soft jaw fixture, a mirror image of the outside profile from above
2. Profile OD to Thread Major Dia
3. Pocket hole
4. Face to final length rinse repeat for 50 parts
5. Change to chamfer tool
6. Chamfer as needed rinse repeat for 50 parts
7. Change to thread mill, thread rinse repeat for 50 parts

Holes
Fixture, Spot drill, Drill, Hand chamfer while the next part is drilling.

I just did the above operations on a batch of parts, less the thread milling and the hex broach.

Bottom line, Tormach 1100 will work fine. Forget the Rapid Turn, buy the ATC instead. The Rapid Turn takes a maximum 25.4 mm bar through the spindle anyway.

[SCzEngrgGroup]

Yeah, you can interpolate the "turned" features, but you're not going to get anywhere even in the same neighborhood as a 32 Ra surface finish on those surfaces with a Tormach, which is why I didn't suggest that.

Regards,
Ray L.

[Steve Seebold]

What price point do you need to be near?

[Jim Dawson]

Yeah, you can interpolate the "turned" features, but you're not going to get anywhere even in the same neighborhood as a 32 Ra surface finish on those surfaces with a Tormach, which is why I didn't suggest that.

Regards,
Ray L.

I didn't realize that. Maybe a bit heavier servo driven machine would be in order then. Or a CNC lathe with live tooling.

[rdsi]

I would run it on a lathe first using the collet closer and a bar puller. This way you eliminate any blank prep & automate all the turning ops. The lathe would complete the bottom threaded portion, the final OD and it’s chamfers leaving a slightly tapered cylinder, with a top radius, for the upper half.

Then I would fabricate a threaded fixture plate/bar to hold a bunch of these on the mill to complete the top features.

The two little holes could be handled several different ways but my first approach would be to have the fixture plate/bar so that it could be mounted in one of two positions that are rotated by 90 degrees.

The only special tooling would be a tapered end mill & rotary broach. I can’t really tell from the pictures but the top valley walls have a chamfer on them that may require another tapered end mill.

Yeah, the fixture may need some features to keep the parts from rotating out while machining. You might be able to design the CAM program to keep the cutting forces the right way. In either case I think it’s very doable.

Just some thoughts ...

[motoeng]

What price point do you need to be near?

If you're referring to the machine, $15-$20K, tooling included. Ideally, I wish I could afford a separate lathe and a mini mill. It would be nice if Haas offered the educational price on the mini mill to the hobbyist. I can afford a $19K machine, especially with those specs, but at the regular introductory price of about $30K, it's a little out of reach at the moment.

[GLCarlson]

If you're referring to the machine, $15-$20K, tooling included. Ideally, I wish I could afford a separate lathe and a mini mill. It would be nice if Haas offered the educational price on the mini mill to the hobbyist. I can afford a $19K machine, especially with those specs, but at the regular introductory price of about $30K, it's a little out of reach at the moment.

Moto- several members of the forum are known to do small runs of parts. Steve S is one. You might look back through old posts and identify the half-dozen or so who are experienced, equipped, and interested and then have some side discussions with one or more of them. At the least, you'll learn a lot. You may find a better supplier, and even someone who could help you move the product in house eventually.

[motoeng]

I would run it on a lathe first using the collet closer and a bar puller. This way you eliminate any blank prep & automate all the turning ops. The lathe would complete the bottom threaded portion, the final OD and it’s chamfers leaving a slightly tapered cylinder, with a top radius, for the upper half.

Then I would fabricate a threaded fixture plate/bar to hold a bunch of these on the mill to complete the top features.

Thx rdsi. My current supplier turns the part first then switches to the vertical ops. I've received one of the turned blanks before to confirm this.

If I decided on the Rapid Turn, the OD of the part is too big for any of the collets so I guess I'd be stuck using a three jaw chuck in that. It seems like I might have a lot of material waste using that method though if you're not able to feed the stock down into the lathe and just pull out some more for the next piece. I'm not sure if that's how it works when you're using a collet on the machine, but would assume so.

On the largest outer diameter of the part, there are three superficial marks equidistant from one another, indicating they fixtured it in a 3 jaw for at least some of the vertical machining, if not all of it. There's not a lot to grab onto for that diameter though, so I'm not sure how you would stabilize it unless you put a blank underneath to support the bottom of the part while it's in the chuck. Not even sure if what I'm saying is possible to do in a chuck.

I've thought about having some sort of fixture plate where you could screw a bunch of these in, but it seems like there would just be too much slop between the mating thread surfaces for the parts to stay perfectly still during machining. Then you'd have them wanting to unscrew. Would be a huge time saver if something like that could be constructed though.

[motoeng]

Moto- several members of the forum are known to do small runs of parts. Steve S is one.

Gotcha - so Steve was likely referring to piece price. Duly noted!

[Steve Seebold]

Gotcha - so Steve was likely referring to piece price. Duly noted!

If you are looking for the absolute rock bottom piece price, as much as I hate to say it, a Tormach is not going to be the machine for you.

There are lots of others out there. One particular is from Haas. I don't remember the model number but it's starts at $195,000.00. I've seen it run and it would run the milled portion of this part in about 3 minutes or less.

[rdsi]

The parts probably look something like this after the lathe OP.



My first thought is that you might be able to get away with screwing them into a fixture plate. The parts will cinch-up against the mating surfaces & if your CAM program makes all it’s cuts such that the forces are all clockwise that might be enough that they stay put. Otherwise, the plate would need some more features – not too difficult…

Yeah, I see your OD is 29mm and that’s not going to happen with a 5C collet & bar puller. I think the max here is 1 1/6” or about 27mm. With the 3-jaw chuck on my Slant-Pro I can get 1.5” through the spindle. Unless you can make your part a little smaller OD wise you would have to use the 3-jaw chuck and advance the bar stock by hand – at least on the Slant-Pro. There are machines with hydraulic chucks but they’re pretty expensive.

I’m not a fan of the Rapid Turn concept. Just too much work to switch back & forth.

I think it’s doable and that’s why I have a few machines. It’s costly to make prototypes and small lots and that’s where these hobby machines come into play. I’m retired (don’t have to work anymore) but I still like making things.

[motoeng]

Yep - that's exactly what the blank looks like. For what it is, I think the concept of the Rapid Turn is great for those who don't have the funds or space for a second machine.

The setup/breakdown would not be bothersome to me. I've been anodizing my own parts for years and due to lack of space, I don't have a permanent anodizing line setup, so it's an hour for setup and a little less for breakdown each time I run a batch of parts. Horribly inefficient, but it's what I have to do to get the results I'm after.

Would you happen to know how much material would need to be held inside the chuck in order to machine this part, or are there specs somewhere that tell you this? I'm wondering how much waste I would have when turning each one.

[SCzEngrgGroup]

My first thought is that you might be able to get away with screwing them into a fixture plate. The parts will cinch-up against the mating surfaces & if your CAM program makes all it’s cuts such that the forces are all clockwise that might be enough that they stay put. Otherwise, the plate would need some more features – not too difficult…

It has little or nothing to do with the CAM. It would require CCW-turning (i.e. - "left-handed") tools.

Regards,
Ray L.