.50 thru hole with compound angle on manuall mill help??

fettersp · May 4, 2020

i'm having issues on how to setup for the thru hole on this part. the part looked easy at first until i got to the last part of the job. I have my mill kicked to 30 degrees and have a sine bar kicked to 38 degrees, part had to be flipped over to sit on the vice correctly and the hole has to start at the break thru point because the other way will make me drill through my sine bar. I have no clue to to edge find or indicate to get the right spot for the thru hole. any advice would be of great help. the tolerances are +- .0005.

carlherrnstein · May 4, 2020

It's sort of difficult to understand what is going on there. I try my best to avoid tipping the mill head because you lose your capacity to edge find.

I think you need to drill a compound angle. I would set the head straight, tram it, set the vice at one angle and make a sacrificial angle block to get the other one. You will need to figure out the position of the hole from something you can edge find.

Larry Dickman · May 4, 2020

I always use a tooling ball to find location. Dead nuts every time

implmex · May 4, 2020

Hi fettersp:
At the risk of sounding like a complete dickhead, I have no idea what that scribble you've put up as a drawing is supposed to represent.
Do you have any other information you can give us?
How about photos of the setup you are planning on the actual mill?

Moving on to the ambition to position a hole on a manual mill on a compound angle to within a thou (+/- 0.0005"); how do you propose to interrogate it to see if it's where you hope it to be?
What are your datums from which you intend to measure?
How confident are you that your mill is "kicked over" to exactly the correct angle.
Will you locate off a tooling ball, or a scribed line or a touch with a cylindrical pin or ???
Do you have room to put in the hole close to it's desired location and then adjust the outsides of the part to bring it into position?
Do you have the means to mount a tooling ball, position it, verify it, and then pick it up and bore on that location without shifting the spindle axis relative to the ball when you run the table up and down to get the indicator and tooling ball out and the boring head into the spindle.

What kind of mill are we even talking about...do you hope to do this on a Bridgeport?
A Moore jig borer?
A cheapo asian import?

The more information you can give us, the more intelligent our response can be; so send us photos and let's see what we're up against.

Cheers

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

SIP6A · May 4, 2020

If I was doing this job I would start with a piece of stock that is machined all over but is bigger than the finished part in all dimensions. I would layout and put the hole in first. I would then machine the part to fit the location of the hole. I don't know what you have to work with in the way of measuring tools and machinery. I could do this in my shop with a bridgeport. A sine table and a set of gage blocks.

PS: I wish I got drawings that nice to make some of the stuff I make.

gbent · May 4, 2020

I'm with Marcus about not knowing what your sketch represents. The views do not agree with my drawing knowledge.

If true position of the hole is .0010, one shot, that is a couple of hundred dollar hole. There will be serious discussion about acceptance criteria as well. Yes, I could and have done similar. But its not a fun afternoon.

Booze Daily · May 4, 2020

SIP6A said:
...I would start with a piece of stock that is machined all over but is bigger than the finished part in all dimensions. I would layout and put the hole in first. I would then machine the part to fit the location of the hole.

This. But how are you going to check it?

SIP6A · May 4, 2020

Booze Daily said:
This. But how are you going to check it?

You would machine a piece of stock say .100 larger on all dimensions. You would then put the hole in as close as you could using what you have to work with. Then you would press a gauge pin in and set it up on a sine plate for the angle you wanted to measure. You indicate across the pin and you will be out some number lets say .005 on one end and .0000 on the other end. You then do the math and set up the part to machine off an amount so when you put the part back on the sine plate it now measures .0000 and .0000 you repeat this with all the other surfaces on the part.

Now I do understand that this involves more work than just some typing and hitting the go button but the unfortunate truth is sometimes you just have to do some actual work.

fettersp · May 4, 2020

I have never used a ball touch off tool. I only have the cylindrical touch off tools.
I'm pretty confiden in the two angles that I have kicked off. The picture of the mill is how I have it set up so far but I'm not sure on how to touch it off with a cylindrical touch tool. My scribble was pretty much the drawing I was given I posted a pic of the dimensions I scribbled. I mean I dont Carr iv your a sick to me, as long as I learn something. This was a part my dad accepted before passing away and he was the master of odd stuff like this.

Cole2534 · May 4, 2020

Larry Dickman said:
I always use a tooling ball to find location. Dead nuts every time

Would you be so kind as to explain how this works. I get that the ball is an easy to locate datum, but I don't see how it really tells you anything.

Sent from my SM-G930R4 using Tapatalk

gbent · May 4, 2020

Tooling balls are typically installed in the part in the flat, non rotated orientation. A tooling ball gives you a point in space you can pick up from an angle. You make a layout to determine where you want your point in space. Sometimes you make a dummy part with a tooling ball similar to the real part and swap the parts in your fixture after picking up the location. Other times you put tooling holes in the finished part where they are out of the way. If the part is large enough, you can put the tooling ball hole in the hole that is machined away.

You can get tooling balls with shanks that can be positioned for height, or shouldered tooling balls with a precise dimension from the locating shoulder to the centerline of the ball.

With tooling balls, always work off the centerline of the ball. Don't mistake the top surface of the ball as the correct place to touch off tooling height.

Larry Dickman · May 5, 2020

Cole2534 said:
Would you be so kind as to explain how this works. I get that the ball is an easy to locate datum, but I don't see how it really tells you anything.

Sent from my SM-G930R4 using Tapatalk

what gbent said above. If there's no convenient place to mount the ball on the part, you can mount it on the sine plate. So you can pick up the location of the ball at 0 deg, then calculate where your bore should be at 38 deg. And like gbent said, always work to the center of the ball.

Cole2534 · May 5, 2020

gbent said:
Tooling balls are typically installed in the part in the flat, non rotated orientation. A tooling ball gives you a point in space you can pick up from an angle. You make a layout to determine where you want your point in space. Sometimes you make a dummy part with a tooling ball similar to the real part and swap the parts in your fixture after picking up the location. Other times you put tooling holes in the finished part where they are out of the way. If the part is large enough, you can put the tooling ball hole in the hole that is machined away.

You can get tooling balls with shanks that can be positioned for height, or shouldered tooling balls with a precise dimension from the locating shoulder to the centerline of the ball.

With tooling balls, always work off the centerline of the ball. Don't mistake the top surface of the ball as the correct place to touch off tooling height.

Thank you

Larry Dickman said:
what gbent said above. If there's no convenient place to mount the ball on the part, you can mount it on the sine plate. So you can pick up the location of the ball at 0 deg, then calculate where your bore should be at 38 deg. And like gbent said, always work to the center of the ball.

Thank you

I watched a youtube vid last night on how they're used and it brought it together better for me. They'd be a good place to practice your trig.

implmex · May 5, 2020

Hi again fettersp:
Another question: how did you decide this hole needed to be on location to +/- 0.0005"?
There does not appear to be a notation on the portion of the drawing we can see; the hole diameter is called out to only two decimal places and there are no tolerances on the location callouts that I can see either.
Is there a notation in the title block?
Is there a note on another view?
Did the customer make the demand verbally?
Did you decide, based on the function, that you needed this very ambitious precision to make the assembly work?

I ask because certifying to this precision and making the part to this precision is an extraordinary undertaking if all you have is a Bridgeport and a caliper and maybe a half thou indicator.
An experienced toolmaker can probably pull this off, but as a previous poster pointed out, this is going to be one helluvan expensive hole even for a guy with decades of experience.

Cheers

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

guest · May 5, 2020

fettersp said:
...I have my mill kicked to 30 degrees and have a sine bar kicked to 38 degrees,

Recommend you find a tutorial on compound angles, you do not set them up that way.

The first angle changes the second one.

fettersp · May 5, 2020

I think that I figured it out. I ended up laying the part flat and turning the mills head to 38 degrees while the vice is turned to 30 degrees. I also scribed the location of the dimension and made a small indent in the spot where the axises meet, then used a needle wobbler to zero that spot.(I'm not sure what exactly the tool is called.). After that I ended up using a carbide endmill since the drills kept wanting to flex on me.
All the parts are within tolerance and ready for heat treat now.
I would upload a picture of the set up but the forum is just letting me click upload and not doing anything.
I'm still learning how to use a mill as I am more of a cnc lathe person.

implmex · May 5, 2020

Hi again fettersp:
I'm glad it worked out satisfactorily for you, but I'm having a very hard time believing you got it to within your stated requirements using the method you describe.
How did you measure it to be sure it is good?

Cheers

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

carlherrnstein · May 5, 2020

He said the words "heat treat" it's been my experience that when something goes out for heat treat it will come back distorted. Chances are the tolerances don't need to be that tight.

guest · May 5, 2020

fettersp said:
I think that I figured it out. I ended up laying the part flat and turning the mills head to 38 degrees while the vice is turned to 30 degrees.

Well, that is not a compound angle. That's just a 38 degree hole that happens to be rotated 30 degrees off the centerline axis of your part.

A compound angle is when your angle is on 2 planes. Your hole is 38 degrees on one axis, and 90 degrees on the other axis. It's just an angled hole, nothing more.

I do a cable sheave that gets a hole on a compound angle. The cable enters on the front of the sheave and exits in the center of the groove at a shallow angle so the cable does not make a hard bend when it winds onto the sheave. This hole has to exit on the center of the groove, so the head of the mill is kicked over to one side, and nodded in the other axis.

Setting up a compound angle is more involved than just calculating the SIN of each angle. Suburban has a calculator.

SUBURBAN TOOL, INC. - How To Use A Compound Sine Plate

fettersp · May 5, 2020

I measured it with calipers to the middle of the oplyptical. I showed the customer them when I was delivering different parts. He measured the same way I did and said it's good so I didnt think much of it after that and sent it to heat treat. The material is oil hardened and in my experiance qith oil hardened materials it doesnt change much. But I am more curious about tool balls now.

.50 thru hole with compound angle on manuall mill help??

Aluminum

Aluminum

Titanium

Diamond

Titanium

Diamond

Titanium

Titanium

Aluminum

Diamond

Diamond

Titanium

Diamond

Diamond

guest

Guest

Aluminum

Diamond

Aluminum

guest

Guest

Aluminum

Similar threads