What's new
What's new

Work holding question from inexperienced guy.

Aegir

Aluminum
Joined
Feb 21, 2018
OK, so if you came to this question from the tittle to help out someone with little experience, I thank you in advance.
So I am happy with feed and speeds etc, but I am having some issues making a particular part. It is 316 stainless, so I am taking fairly easy cuts. I mention that only in relation to the forces being put on the part for holding it.
P3213487.jpg
P3043313.jpg


Ignore the click ring and the glass of course, on the first picture.
I do not have a probe on my milling machine and so have attempted to first prep some stock from a solid piece of round bar , pre cut to a few mm thicker than I need in my vice and machine out the seat where the glass goes (in that first picture) and then a hole through the middle so I can use an expanding clamp and tighten the bolt down.

I did add a feature to the drawing to try and locate the part onto another expanding clamp when I flip it over and then planned to machine that feature out near the end. It has to be located perfectly of course, or it is just not going to work out. I made a mistake on the clamp , so have not been able to use that and have to order some online.
I still need to then take the case after I have machined the inside steps, which include three different dimeters inside from the back, a slot and threads where the case back will screw on, the top side done and getting that lug profile perfect (where the strap attaches) to then machine out the area on the winding crown and drill the holes for the that and the straps.


So I thought that before I order more clamps (not the cheapest things) I would ask here, how others might make this part. It is not a one off, but will be made in very low volume though.
I have no access to a lathe or probe at this time and what I need to do is prove I can actually make this, before I can invest in another machine, which I am ready to do once I have made several of these parts and they are up to spec.

So given that information, can I ask how you would attack this part?
 
Last edited:
One realy crude but works for me way has been as simple as a peg in a tool holder, drop part on clamp manderal (my case it was a 3 jaw chuck external jaws, then have the spindle bring the Peg into a previously milled V, programmed pauses, tighten chuck and hay presto you have picked up the angular rotation. Your winder Bumps look like they could work well for this technique. Other option can be as simple as a flip over stop that you load rotate against then flip out the way.

probes are usefull don't get me wrong, but they take time, faster is always better and nothing beats the simplicity of a stop.
 
QT Op:[I have no access to a lathe or probe at this time and...}
So what machine are you using to make prototype? looks like a tough part to make.. Is a solid bar stock the best starting position? Parting off is a time consumer.

QT Op: [Work holding question from inexperienced guy.] That part from an inexperienced guy...What?
 
I have a Mill only.
So far I have machined the underside with nice profiles to those lugs , and have also ''eyed'' in the second op and while not really lined up perfectly, have still managed to see that the machine can make that profile.
The stock was time consuming and a waste , including tools, so I now have bought pieces of round bar , cut about 5mm thicker than I need and the bar was larger in diameter as well, so some metal to remove, but not too much. This part is one of approx 5 I am trying to produce, but certainly the hardest, so I put that one up.
 
One realy crude but works for me way has been as simple as a peg in a tool holder, drop part on clamp manderal (my case it was a 3 jaw chuck external jaws, then have the spindle bring the Peg into a previously milled V, programmed pauses, tighten chuck and hay presto you have picked up the angular rotation. Your winder Bumps look like they could work well for this technique. Other option can be as simple as a flip over stop that you load rotate against then flip out the way.

probes are usefull don't get me wrong, but they take time, faster is always better and nothing beats the simplicity of a stop.

You mean like a vice stop sort of thing?
 
Hi Aegir:
I remember this part from a thread you had running about investing in a new machine several months ago.
So are you still making these on your Wabeco or did you spring for the Haas?
I assume you still do not have a lathe, so these are going to be 100% milled?

Moving on to your question for this thread; I would cut these from a square bar that has been milled or ground all over to be accurately square and of a known size.
The bar should be long enough to make a whole bunch like cutting off sausage slices but not so long as to cause problems milling on the end of it.
4" tall or so is probably a good length for a small CNC mill.

I'd poke in all the side holes first, using a simple milling vise, then stand it up on end and mill everything I can from the top.
I'd slice off the half completed part on the bandsaw, and set up the block again to make another by dropping the Z axis offset or propping up the block on parallels.

I'd buy a small 6 jaw lathe chuck with 2 piece jaws and bolt it to a square plate so it can easily go on the mill.
I'd make soft jaws for the chuck and mill a pocket in it to hold the half completed part bottom up (that's why it's important that it's a 2 piece jaw style chuck)
I'd mill the second side using the soft jaws to locate the part(s) radially and axially.

Sounds simple, doesn't it?

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
 
You mean like a vice stop sort of thing?

Nah, what he means is imagine a dowel pin in a toolholder. You start your program and the tool goes to a said position, and you do a M00. You put your part in your fixture and rotate it to touch the dowel. This way you know where your part is aligned. You then hit your cycle start and it does it's thing cutting it.

It is a really smart suggestion from adama, you are using your machine to align the part so that you know that they are all aligned exactly the same. This way you could use your idea of an expanding mandrel.

I like what Marcus suggested too. As long as you can accurately get your heights right after each saw it should be good especially since you are not doing big quantities.

Is there any way that you could leave a bit on the outside from the first op so that you could take a light cut in the second op to make sure that all the grooves and outside are aligned? I understand that it is a complex shape so trying to reach the underside of the "tangs" (sorry about my terminology) might be a pain.

Damn nice work by the way!
 
Aegir - you do realize that you can do many lathe operations in a milling machine, right? (And this part is well suited to some of these techniques.)

Note that above when Implex talks about a 6-jaw chuck, the intent is that you will fasten it to the table of the milling machine - you are using it as a kind of vise.

To do "lathe" operations you will need a boring head, and both right-handed and left-handed boring bars that fit said head. You use one of them to make inside diameters - conventional boring (I think this is the right handed one but I always have to lay it out to be sure.) You can use opposite handed tool to make *outside* diameters - which will be important shortly. (The reason you can't just go backwards on the spindle with the same handed boring tool is that most boring heads are screwed on their arbors and will come off the tool holder.)

You can also put the workpiece into something like an ER collet, spin it in the spindle, and then use a conventional lathe tool in a vise to turn that part - that works OK for short parts (in my experience anyway) but the techniques with the boring head are more useful for the part at hand.

OK, so you have made your stock Very Square, and can thus hold it upright in a well known configuration (meaning you know where zero is) and mill (and bore it) correctly for the first side. You can also turn it on its side (or mutiple sides) and know where zero is (because the stock is very square.)

In addition you make a fixture part that has a boss (cylinder sticking up), which you have "turned" on your mill with a boring head. That boss is a close fit to the ID of your part, and so if you flip the part over and slide it down the boss, you are very well centered.

Sticking down from that boss is some shape that is handy for what you are doing. (Close fit to the thru-hole on a chuck, fits a jig plate that goes in a vise with soft jaws that orient the part, etc.)

Now - as practical matter you will want a good locating solution - of which a renishaw (or similar) probe is a great example. But don't be afraid of things like 3-d tester. (Sometimes called a 3d-taster)

The key point is these give you XY and Z, are generally rather cheaper than adding a probe to a CNC machine, and are easy to use.

I could not find this on Australian amazon, but that may be due to error on my part:
TSCHORN 3D-Tester SAVEplus - Model: 163B5I: Amazon.com: Industrial & Scientific

Haimer is a big name in these as well:
Haimer Search
 
My approach would be similar to Marcus's except I'd start with round stock just big enough to give you enough stock for the finished periphery. Milling machine for sure. I'd use an indexing head mounted collet chuck or 6-jaw. You'd need two separate setups unless you had a trunnion type setup. Use that to hold the round while machining 5 sides complete, then cut off like Marcus suggests. Make a fixture plate or expanding mandrel setup to clamp the parts with the unfinished side up and finish that.
 
Hi eKretz:
How about starting with round bar and milling four flats so you can still index it in the vise easily.

I know where you're coming from using an indexing head; and on a reasonable machine if there are lots to make, your way is the obvious way: but f the OP still is using his little Wabeco mill, he's going to have rigidity issues with an indexer that's light enough for such a small mill to still drive around without overloading the table.
He's only got a few side operations so for the few watch casings he wants to make per month (I'm referencing his previous thread now) keeping it simple and rigid is a big benefit, besides the economy factor in not having to buy an indexer or tool it up.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
 
You mean like a vice stop sort of thing?

Yes have used a pivot out the way type vice stop too for this sort of stuff as well as the pin in the actual machine spindle, certain parts just lend themselves to different strategies, there's no right or wrong on this kinda stuff. A lot of it is limited to your imagination and what you already have. key thing is to keep the fixture and machine clean at part change over. People hate airlines, but IMHO fiddly crap were you need to index it like were discussing here you need everything proper clean and dry because even just a small chip in tjed way and you lose the part.
 
Hi Aegir:
I remember this part from a thread you had running about investing in a new machine several months ago.
So are you still making these on your Wabeco or did you spring for the Haas?
I assume you still do not have a lathe, so these are going to be 100% milled?

Moving on to your question for this thread; I would cut these from a square bar that has been milled or ground all over to be accurately square and of a known size.
The bar should be long enough to make a whole bunch like cutting off sausage slices but not so long as to cause problems milling on the end of it.
4" tall or so is probably a good length for a small CNC mill.

I'd poke in all the side holes first, using a simple milling vise, then stand it up on end and mill everything I can from the top.
I'd slice off the half completed part on the bandsaw, and set up the block again to make another by dropping the Z axis offset or propping up the block on parallels.

I'd buy a small 6 jaw lathe chuck with 2 piece jaws and bolt it to a square plate so it can easily go on the mill.
I'd make soft jaws for the chuck and mill a pocket in it to hold the half completed part bottom up (that's why it's important that it's a 2 piece jaw style chuck)
I'd mill the second side using the soft jaws to locate the part(s) radially and axially.

Sounds simple, doesn't it?

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

I had made an agreement (wife) that before I purchased the Robodrill I settled on, that I would show her 1 finished case. That is going to be brand new, so no money for a lathe
 
So several different ideas on how to get this done in there and thank you for the replies.
I still only have the Wabeco mill and entered into a bargain with my wife, that if I can show her a finished part that fits together (case back, case and bezel) that also has the final surface finish, I can have the Robodrill.
So that is fair, as this is all in a home garage, not a shop.

So square bar makes sense to me, to put the holes in first, at least I can find a reference then.

My thinking so far, was to face down sections of round bar to 1mm thicker than the finished part with the part already on the expansion clamp, meaning it is square to the fixture. That was my thought anyway.
Then rough out the part, because I do not need to locate it in the first operation, as it will machine from round. Then I am left with a case that is 80% done and need to flip it over and machine the top. That is where I have come unstuck and I had no idea how I was going to get the holes and machine out the winding crown area lined up as the third and final operation.

I will read through these ideas again, and see if I can not make parts on them work with my existing tools and when I buy the Robodrill I am happy to invest in other work holding devices. A 6 jaw chuck to add now sounds a little costly , as I have a real concern that I am not up to the task. At the end of the day, I am a commercial diver trying to be a self taught machinist off Youtube and forums etc. Worked ok, but no substitute for doing it properly
 
Yes have used a pivot out the way type vice stop too for this sort of stuff as well as the pin in the actual machine spindle, certain parts just lend themselves to different strategies, there's no right or wrong on this kinda stuff. A lot of it is limited to your imagination and what you already have. key thing is to keep the fixture and machine clean at part change over. People hate airlines, but IMHO fiddly crap were you need to index it like were discussing here you need everything proper clean and dry because even just a small chip in tjed way and you lose the part.

I was trying to use the spindle with a tool upside down in the collet to get the smooth area. I did also consider using a vice stop like you say, but on a pallet changer so I can set them up on a work bench and contacted pro-vice I think it was and he told me it was not suitable. I think that might be over complicating it though. Would be nice if I can take a system that works from this machine to a new industrial machine as well, so I am not experimenting all over again. I did see this after you termed it ''flip stop'' .
CMS - Adjustable Flip Stop

There might be a combination of things I can take from this thread and make it work. Doing the holes first now seems like the next step
 
Hi Aegir:
I remember this part from a thread you had running about investing in a new machine several months ago.
So are you still making these on your Wabeco or did you spring for the Haas?
I assume you still do not have a lathe, so these are going to be 100% milled?

Moving on to your question for this thread; I would cut these from a square bar that has been milled or ground all over to be accurately square and of a known size.
The bar should be long enough to make a whole bunch like cutting off sausage slices but not so long as to cause problems milling on the end of it.
4" tall or so is probably a good length for a small CNC mill.

I'd poke in all the side holes first, using a simple milling vise, then stand it up on end and mill everything I can from the top.
I'd slice off the half completed part on the bandsaw, and set up the block again to make another by dropping the Z axis offset or propping up the block on parallels.

I'd buy a small 6 jaw lathe chuck with 2 piece jaws and bolt it to a square plate so it can easily go on the mill.
I'd make soft jaws for the chuck and mill a pocket in it to hold the half completed part bottom up (that's why it's important that it's a 2 piece jaw style chuck)
I'd mill the second side using the soft jaws to locate the part(s) radially and axially.

Sounds simple, doesn't it?

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

No, it does not sound simple!
If I was to use this chuck 6-JAW SELF-CENTERING SCROLL CHUCK 3865-125 - BISON-BIAL S.A.
wouldn't I be machining through the jaws to get to the very bottom of the lugs when ding that profile from the top down? I keep looking at this , not seeing how I could hold the part in two different diameters without machining half these jaws off as I go. I know I am not looking at it right.
I do have a 4th axis for this machine, though never set it up, nor have I ever made tool paths in Fusion 360 for it.
I would have to mill the squares myself , because the budget would not allow to have an outside company grind them. Not in Australia anyway!
 
Hi eKretz:
How about starting with round bar and milling four flats so you can still index it in the vise easily.

I know where you're coming from using an indexing head; and on a reasonable machine if there are lots to make, your way is the obvious way: but f the OP still is using his little Wabeco mill, he's going to have rigidity issues with an indexer that's light enough for such a small mill to still drive around without overloading the table.
He's only got a few side operations so for the few watch casings he wants to make per month (I'm referencing his previous thread now) keeping it simple and rigid is a big benefit, besides the economy factor in not having to buy an indexer or tool it up.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Good call, I missed the previous thread and other limitations.
 
No, it does not sound simple!
If I was to use this chuck 6-JAW SELF-CENTERING SCROLL CHUCK 3865-125 - BISON-BIAL S.A.
wouldn't I be machining through the jaws to get to the very bottom of the lugs when ding that profile from the top down? I keep looking at this , not seeing how I could hold the part in two different diameters without machining half these jaws off as I go. I know I am not looking at it right.
I do have a 4th axis for this machine, though never set it up, nor have I ever made tool paths in Fusion 360 for it.
I would have to mill the squares myself , because the budget would not allow to have an outside company grind them. Not in Australia anyway!

That is why he said to use soft jaws. You can machine them into the shape you need before working on the parts so that they register correctly where you need them to but are otherwise out of the way.
 
That is why he said to use soft jaws. You can machine them into the shape you need before working on the parts so that they register correctly where you need them to but are otherwise out of the way.

I understood that bit, but looking at a picture of the chuck I cant see how I would machine the part top side up in the second picture I posted, without machining large parts of the jaws away in the process to get to the bottom, making them not function as intended.
I have limited experience using a chuck, and never saw a two piece jaw one before.
So if I buy it and do the operation with the lugs facing up , fixed in the silhouette I machined for that purpose, when I flip the part over there does not seem to be the clearance.
Or do those soft jaws extend quite some distance up?
 
I understood that bit, but looking at a picture of the chuck I cant see how I would machine the part top side up in the second picture I posted, without machining large parts of the jaws away in the process to get to the bottom, making them not function as intended.
I have limited experience using a chuck, and never saw a two piece jaw one before.
So if I buy it and do the operation with the lugs facing up , fixed in the silhouette I machined for that purpose, when I flip the part over there does not seem to be the clearance.
Or do those soft jaws extend quite some distance up?

He is talking about using the chuck with custom soft jaws for machining the backside AFTER having machined the first half (as much as can be accessed on the blank held in a vise) and cutting it off with a bandsaw.

The custom soft jaws are machined to grip the allready machined surfaces.
 
He is talking about using the chuck with custom soft jaws for machining the backside AFTER having machined the first half (as much as can be accessed on the blank held in a vise) and cutting it off with a bandsaw.

The custom soft jaws are machined to grip the allready machined surfaces.

So only the one operation on those jaws then, leaving material around the bottom so there is a corner to pick up the orientation of the part once it is transferred , if I am getting it.
 








 
Back
Top