What's new
What's new

Achieving seamless profile when contouring on secondary operation

I generally use the full depth in first set up then deck off base. You can probe or swing an indicator and get virtually no blend but you need to machine equal depths from top and bottom or tool pressure alone will give a small mismatch. In Australia where we don't have the material size selections that most do I would single point bore and pick up the hole from the other side. Too save time you can use the boring cycle and back bore the bare minimum for clean up so only your indicating point is true. I would make the boring tool so I have the least offset mass and can spin it faster than a boring head.
 
Use dovetail jaws holding about .07 material go the whole distance on op 1 flip it and deck it off. No extra material needed it looked like in the pic he had .250 of stock
Don

I haven't tried those yet, in my experience, Dovetail cutters are slow and annoying so I avoid them unless I need a dovetail feature in a part. Do you use these for steel too?

Sorry man I don't follow. Why add .250"...this adds a lot of cost to the already pricey material plus some additional tooling costs as I'd need 2.5" LOC tools.

Adding stock is still cheaper than trying to solve this problem by any other means, that's why most of us will do it whenever we can. It's easy to implement, easy to calculate cost and guaranteed to get the results you need the first time.

It does suck wasting material but that is still cheaper than wasting hours - spending a dollar to save a dime if you know what I mean.

Do you already have all of the material and tooling ordered for this job? Have you already run a significant number through op1?

If so, any solution may need to take that into consideration; unless you can buy tooling and material again and save the other stuff for a different job. We've all been there, either way it's a "remember this for next time and don't do it again" sort of learning experience. It happens to the best of us lol.
 
I haven't tried those yet, in my experience, Dovetail cutters are slow and annoying so I avoid them unless I need a dovetail feature in a part.

I believe he's talking about these, Mr Bigballs Machine ...

IMG_0452.jpg

I'm kind of amazed at how much you can remove holding the part by basically nothing, too. Little teeny cuts I guess. Your Devlieg probably can't even move in those small amounts :)

"Cut ? You call that a cut ? What's wrong wit chew, jose ! Take off some metal before I die of boredom !" :D
 
Where are you located? Someone in your area probably has a good source for you to get your material from if you think that chunk is expensive.

When setting a 2nd op zero with grip material on top, use a gauge block in between the probe and finished surface then shift gauge block amount.
 
I believe he's talking about these, Mr Bigballs Machine ...

View attachment 406546

I'm kind of amazed at how much you can remove holding the part by basically nothing, too. Little teeny cuts I guess. Your Devlieg probably can't even move in those small amounts :)

"Cut ? You call that a cut ? What's wrong wit chew, jose ! Take off some metal before I die of boredom !" :D

😂 oh, that would make more sense. I have seen dovetail jaws where all the material has to be prepared with dovetails before hand, it was on some fancy youtube 5 axis stuff though.

I usually just clamp on 1/8", give it a whack with the dead blow then feed er' the beans. I'm too impatient for light cuts. These days I just input the tool data and material on my FSwizard app and run what it tells me - except for helix boring. I printed out a thread from the mastercam forum where a few of those guys came up with perfectly usable equations to figure out ramp angle and such.

I don't get to run Devlieg's much anymore 😕. It's ok though, just like the old Warner Swasey's; it keeps it fun on the rare occasion that I'm the guy for the task.

If I had the money, I'd have two machine shops; one for business and one for pleasure 😁.

Edit: Lol, I just realized how similar the words impatient and impotent appear to each other, stupid auto correct.
 
Last edited:
I’d start with one surface perpendicular to the bore. Then I’d drill and ream, if necessary, and do the twelve pouches. Then I’d flip the part to machine the opposite flat. Then I’d put in a mandrel, clamp the mandrel between a dividing head and counterhead (spacers, dog) in a horizontal setup. Then I’d machine the outer form in one movement. It could be feasible to take the chamfers with under a combination of cutters.

It can be done by CNC equipment, even on a lathe with live A axis. No need to worry about hole location when locating work by the bore
 
Below is the most up to date methodology as proven by countless young machinists.

Step 1. Grow a long beard.
Step 2. Get full sleeve tattoos.
Step 3. 3d print it.
Step 4. Start a YouTube channel and tell everyone how it should be done.

I may have the sequence wrong.
 
I've done some experimenting using my Blum spindle probe for blending surfaces after flipping. My experience is that if I drill a hole with an end mill, then measure it's location, it's usually quite a lot of microns away from where it should be. (In aluminulium)

If I run the end mill in and out a few times then the centre is quite a bit closer, but still wanders around

My new technique for fixtures is to drill a locating hole, then set the zero point to wherever the hole measures... Then finish the fixture. At least that way I can remeasure accurately

However measuring flat surfaces works way better! If you can cut all the way through and make a flat spot then this measures way better! I guess this makes sense in that small deviations of roundness amplify deviations measuring centres of round holes?

So if I need to very accurately align an op for a flip I find a way to machine a flat to measure X and Y. Note you don't need to measure the actual part, you can create a flat anywhere you can measure. Also you can use the hole to get a rough location, then rough off enough material to get close enough to measure cut material (you just need to get close enough that the ball if the stylus can measure past whatever top hat is left). So using the probe I can measure the stock, rough the part, then measure exactly and finish. Obviously this is more practical with an automated probe!

Soft jaws would seem to be the answer for the OP I think?
 
Sorry man I don't follow. Why add .250"...this adds a lot of cost to the already pricey material plus some additional tooling costs as I'd need 2.5" LOC tools.

I've seen long flute carbide drills before but never used them. How do they differ in how they're used?
Since when is 6061 a "pricey" material?
 
Since when is 6061 a "pricey" material?
For me, since right now, I'm just starting this business and the costs are all out of my own pocket until I generate sales / profits. Also, to be competitive in the market I'm in, costs of everything need to be considered.
 
When I flip the part I use gauge block to probe with Haimer from the machined outer surface. Bit fiddly, but gives good results. Just need to remember to deduct the gauge block thcikness.
 
Profile stepping can be mitigated to a large degree by using large corner radius endmills and overlapping a bit.

I generally advocate the extra stock method as it's just easier and the material overhead is usually less than the labour overhead of working with near net stock.

But if the material loss is a big deal, corner radius endmills will help a lot with the step.
 
I'm not so concerned with the complete straightness of the hole as I am the seam. Indicating off of the machined corner (below the raw material edge) instead of the drilled hole might solve this?
It would seem appropriate to zero off the surfaces you want to blend to.
Zeroing off the drilled hole is not going to work well.
Even if was jig ground there is flat, square and parallel of the clamp/locating surfaces to worry about.
 








 
Back
Top