Hole Pattern Problem

[KSky]

I'm not a newbie with my 1100 Series III, but this one has me a bit perplexed. I have a jig (see picture) with 9 holes in a rectangular position. They are cut from front to back with a part I made using fusion 360. The problem is that the center three threads are always too small, in that my test gauge fits great in the outer row of holes but is very snug fit in the center ones. They aren't the last ones cut, and the part of modeled in Fusion and is part of a pattern so I am assuming they are all perfectly modeled the same.

Any clues on where I should look into what's going on? It feels more like a fusion 360 issue, but I thought I might bring it up here.

Similar Threads:

• Need Help!- Bolt Hole Circle Pattern Problem FADAl CNC Mill 88
• Bolt Hole Circle Pattern Problem FADAl CNC Mill 88
• Circle With Bolt hole Pattern
• Need Help!- Need advice from the pros - centering a hole and drilling hole pattern
• Knee Mill Hole Pattern

[Steve Seebold]

How are you putting the holes in? Are you helical milling them with a finish pass? Are you stepping them down with a circular finish pass? Or are you finish boring the holes?

I have learned that I haven't been able to get a hole better than .001 in roundness. If I need it better than that, I'll bore it.

[KSky]

I'm first drilling out to 1/2 and then using a bore operation with a 3/8 carbide end mill. The other holes on the outside are spot on. The threads are cut with a single point thread mill.

[Zetopan]

You should measure each hole ID in the X, Y and the two diagonal directions before threading and record the results. This would let you know if your fit problem is due to out of roundness and specific to the X, Y or diagonal directions. Are you using a finishing pass on the holes? What are your feed rates, etc? As previously mentioned, the roundest holes would be done by boring and not by milling. But thus far I do not see enough information from you to indicate that you need to use boring since we do not yet know the root cause of your non-identical fits.

If you are right at the margin of an interference fit it only takes a fractional mil change to make a big difference between fitting or not fitting, so we (and you) need some data.

[KSky]

Thanks for all the excellent suggestions.

To answer a few questions, The holes are cut using fusion 360's boring operation where the end mill travels in a circle around the inside of the hole. I first drill it out with a 1/2 drill to get rid of as much stock as I can. I don't do a finish pass, perhaps I should have. The outside columns of holes are a very tight fit regardless, so that center column must be off just a very tiny bit.

I am using a three flute carbide end mill, 5000 RPM, 39 IPM cutting feedrate, 0.00262467 in feed per tooth. I know I could push it harder, but this is a fixture plate and I wasn't worried about how long it took. Threads were cut with .03 single point threading tool, also at 5000 rpm, 12 IPM and 0.000588235 in feed per tooth. Do a finish pass here and go slow as I was worried about breaking the bit.

Will make a new one when I get back to the shop and measure along the way and post the results.

Thanks all.

[KSky]

I did some more testing and I have pretty consistently .0006 backlash, sometimes .0005 in the X near the center holes. I measure it by going in one direction until my .00005 dial indicator is sitting on a tic mark, then back using the .0001 jog until the needle moves at all.

Not sure if this is easy to see, but I used some blue to see where the contact was and it's in the Y direction, the blue is mostly intact in the X. It makes it seem like I am missing steps in the Y direction does it not?

[joshetect]

I have a lot more backlash in my Y then X. X is about the same as yours, .0007 and Y is .0021

You'll need to add that info to pathpilot. see post below

http://www.cnczone.com/forums/tormac...ml#post2014660

Also what is your tolerance setting in Fusion for that op? It defaults to .004, I changed mine to .001

[SCzEngrgGroup]

I did some more testing and I have pretty consistently .0006 backlash, sometimes .0005 in the X near the center holes. I measure it by going in one direction until my .00005 dial indicator is sitting on a tic mark, then back using the .0001 jog until the needle moves at all.

Not sure if this is easy to see, but I used some blue to see where the contact was and it's in the Y direction, the blue is mostly intact in the X. It makes it seem like I am missing steps in the Y direction does it not?

If you were losing steps, ALL of the holes would be in the wrong position, not just the wrong size, as lost steps effectively permanently shift your machine position zeros. You are probably just seeing the effects of normal backlash and stiction. This is a fact of life with machines in this class. Getting better than +/-0.001" on ANY single operation is as much a matter of luck as anything else. And the backlash you measure in a static test is only loosely related to the effective backlash that will manifest in actual machining. When machining, there are MANY additional factors at work.

Regards,
Ray L.