Machining long parts that are much longer than your X travel - sugggestions?

I need to do some machining on very long parts (approximately 9' long) which is much longer than the X travel on my CNC machines.

I can run them on an open-sided bed mill so I can hang the parts off side of the machine. My X travel is around 40".

I'm looking to achieve locational tolerances of around +/- 0.05" over the length.

In the past when I needed to make long items like this, I have drilled holes every 3', slid the part over, indicated the hole as a new origin, and repeated as necessary to work my way across the length.

But this time I do not want to poke unnecessary holes all over the part.

Any ideas for different ways to accurately transverse a long part like this?

No holes in the finished part to reference?


I've done plenty long parts on our mills, hanging out the window. Usually has holes or slots to reference, so we can just slide the part over, let the probe update the offset and go to work.

Or if you had enough stock you might be able to add an extra hole in the excess stock, then mill that off after repositioning?

Short of that, come up with some kind of clamp with a reference feature (hole/boss) on it. Mill everything you can, then add the clamp to the part. Measure the reference on the clamp in the current work position. Reposition part, then measure new position of reference. A little math and you know the new offset.

Supper easy with the required tolerance.
Machine the part, take a tool holder with a dowel pin in it.
Position at a low value of X Say X2.00 over the part. M00
Put a small piece (123 block?) on top the part touching the pin. C-clamp, or Kant twist clamp.

Move the spindle to X32.00

Slide part 30" and carefully bring small piece up to contact with the pin..
Clamp.
No need for additional holes, features, or re-indicating.
Fast, Easy, Good enough. .05" No problem.

thesidetalker said:

No holes in the finished part to reference?


I've done plenty long parts on our mills, hanging out the window. Usually has holes or slots to reference, so we can just slide the part over, let the probe update the offset and go to work.

Or if you had enough stock you might be able to add an extra hole in the excess stock, then mill that off after repositioning?

Short of that, come up with some kind of clamp with a reference feature (hole/boss) on it. Mill everything you can, then add the clamp to the part. Measure the reference on the clamp in the current work position. Reposition part, then measure new position of reference. A little math and you know the new offset.

Click to expand...

Exactly as above

I made a 1" wide ring, .005 oversized the bore to the Od of the part, drilled and tapped it then split it. Clamped it to the part and used one of its faces to teach x.

I have some tube manifolds I make that are longer than my travel. Not as long as the 9' but maybe this will help anyway.

I made a spring loaded plunger locator tool (see photo). I put it as one of the tools in my magazine. When I need to index the part I drop it down, loosen the vise, index the part till it drops into an existing hole, retighten, press go.

3t3d said:

Supper easy with the required tolerance.
Machine the part, take a tool holder with a dowel pin in it.
Position at a low value of X Say X2.00 over the part. M00
Put a small piece (123 block?) on top the part touching the pin. C-clamp, or Kant twist clamp.

Move the spindle to X32.00

Slide part 30" and carefully bring small piece up to contact with the pin..
Clamp.
No need for additional holes, features, or re-indicating.
Fast, Easy, Good enough. .05" No problem.

Click to expand...

I've also done similar using a thin plate with a .250 hole reamed in it.

Thanks guys!

I like the ideas to clamp on some sort of stop to the part, and reference the stop. Now I'm saying to myself "why didn't I think of that?"!

I just did this for some 3" round bar with .750 slots. I have 30" in X, but the slots were 38" long. So I would pickup on the edge, machine the first 19", then change to a tool with a .750 gauge pin in it, had another offset saved so I could slide the bars down so the edge of the slot was against the pin. This kept the slot aligned and worked as a work stop, tighten the vises and run the same program again to cut the last 19" of the slot. Worked great.

I have a recurring job of milling long parts. Used to do them on the bridgeport until I got my metal planer mill. Since I got it, my long piece work picked up alot. Not many shops have these capacities.

https://youtu.be/AFHDFf_DhlM

Sent from my rotary dial flip fone

pMetal said:

I need to do some machining on very long parts (approximately 9' long) which is much longer than the X travel on my CNC machines.

I can run them on an open-sided bed mill so I can hang the parts off side of the machine. My X travel is around 40".

I'm looking to achieve locational tolerances of around +/- 0.05" over the length.

In the past when I needed to make long items like this, I have drilled holes every 3', slid the part over, indicated the hole as a new origin, and repeated as necessary to work my way across the length.

But this time I do not want to poke unnecessary holes all over the part.

Any ideas for different ways to accurately transverse a long part like this?

Click to expand...

You could take a reference piece of material machined as a gage known length. Attach a self made clamp to the material and use the known gage as a solid measure from one stop/clamp to the other. It will be as accurate as your ability to clamp and move the stops without adding up error very much.

Not very good. You must concede the real situation and that is whatever you spend ime rigging up it still must be in tolerance. Besides actually machining it what is your function? It is ensuring your part is referenced properly and in tolerance.

You might do different things to accomplish referencing but they all involve referencing. Now if your customer does not want extra hole then you can figure out ways to do it yet it will involve a little bit of thought utilizing what you have to work with and a little bit of determined creativity.

You could weld ears of material on the side of the material. Set it up to machine equally spaced distances of say every thirty six inches and bump those onto a stop you have. Still you must reference the part though precisely.

Picture the I’s as stops of thirty six inches spacing machined one to another milled tac welded stops ground off or machined off at a point of after or during your process.

——————I——————-1————-1————-1————-1————-1————-1

Welding and removing sucks though a stop and a piece of material 36 inches long serves as a spacer between clamps of exactly 36 inches to move.

The Is are basically stops machined or ground off and finished to width at some point.

Actually with a 9 foot long part you would not have to use your 36 inch gage much and depending on how accurately you can attach a clamp as a stop and then move it against a fixed stop it may be well in tolerance. It is a attention to how well you can position your stops. You might even use a feeler gage to make sure any gap is noted.

One start reference point. Gage 36 inches long spaces exactly thirty six inches in between fixed clamp on left to next clamp right. Moving material from right of operator/or duh howdy guy to its left.

Clamp and un clamp home made clamps depending on timing, process and movement. You can use one secure pin stop to bump each position just calculate the movements.

You have to think: If the part is 9' long how are the slot features measured?

I'll bet with a tape measure!

I have some shop made spacers with a hook on one end. I pull it against the end of the part, then touch off the stick and I know I’m exactly 12” from the end.