Two sided part

Hi this is my first post on the forum, so I would like to start by saying Hello to everyone.

I have been working with cnc for a couple of years, I got a grizzly bench top mill with a cnc retrofit off ebay, thinking this would be a good way to teach my self how to run a cnc mill, so latter I could get a bigger mill to help with my business. I have done ok with one sided parts, surface finish is not great, and the tolerance is not good, but it seams to work ok. Three days ago I made a screw less vise and decided to try a two sided part, so I could get a finish on both sides and not cut through my vice. The result has been a headache for days. I need four parts, and last night I ran part seven off.
.Attachment 271224 The biggest thing is a misalignment of the two halves, Iv read that a vice flip is not a great idea but for this close would be fine, but its off by .020. Next after measuring dimensions the x- axis seam to be off by .010-.015 on some, and is within .003 on others, while the y is only off by .002, I have set up indicators and checked for lash, and the ability to return to zero, no visible problems. I have tried changing how I setup and flip the part (indexing from edge, then from center) but it dose the same thing in the same direction. Im starting to beat my head in the wall looking for the problem, dose anyone have any ideas, or things to check?
Attachment 271226
the machine
grizzly g8689 bench top mill
stepper motors with ball screws (already installed)
mach 3 controller
bobcad v25 cad-cam
( just a side question is this a good way to learn?)

Quote:

---

Originally Posted by TheSteelDragon

Hi this is my first post on the forum, so I would like to start by saying Hello to everyone.

I have been working with cnc for a couple of years, I got a grizzly bench top mill with a cnc retrofit off ebay, thinking this would be a good way to teach my self how to run a cnc mill, so latter I could get a bigger mill to help with my business. I have done ok with one sided parts, surface finish is not great, and the tolerance is not good, but it seams to work ok. Three days ago I made a screw less vise and decided to try a two sided part, so I could get a finish on both sides and not cut through my vice. The result has been a headache for days. I need four parts, and last night I ran part seven off.
.Attachment 271224 The biggest thing is a misalignment of the two halves, Iv read that a vice flip is not a great idea but for this close would be fine, but its off by .020. Next after measuring dimensions the x- axis seam to be off by .010-.015 on some, and is within .003 on others, while the y is only off by .002, I have set up indicators and checked for lash, and the ability to return to zero, no visible problems. I have tried changing how I setup and flip the part (indexing from edge, then from center) but it dose the same thing in the same direction. Im starting to beat my head in the wall looking for the problem, dose anyone have any ideas, or things to check?
Attachment 271226
the machine
grizzly g8689 bench top mill
stepper motors with ball screws (already installed)
mach 3 controller
bobcad v25 cad-cam
( just a side question is this a good way to learn?)

---

Use a stop on your vise. Model your vise on youe CAD or CAM. Then when you flip the part, put it against the stop before you program your toolpath.

I should add, referenc 0,0 at the theoretical corner of the stop and vise (the fixed part.)

easiest solution if your tools have enough reach to do it is to buy bigger stock than you need by 1/8" or so, machine the whole part (assuming that your part is a block with a hole in it) flip it over, face off the excess material on side 2. Then you dont need to line anything up and you have that excess material to clamp/not machine

it looks like your losing your reference. what I would do Is drill through the part. then on the second op use an indicator and center on the drilled hole. you maybe a couple thousandths off but you'll be way closer than what I'm seeing in the pics. in your cam software program everything in relation to the center of the hole on the second op.

I'm with louieatienza here. Use a stop on the vise. There is something i'm not seeing here. For you to get to this point and not be able to "flip" the part with continuity. Something is missing. I do this daily without a thought, hitting it within tenth's. I don't see it.

Edit: block prep? Is it square within reason? Offset in the cad/cam proggie? Seems simple to me, I'm misssing it.

I think what's happening is the op is using the same program for each side, problem is referencing the flip. Since material is already removed it might affect the second side. Or the op is not referencing a correct feature on the part. Which is why the stop works well, regardless the shape of each side.

i.e. if the stop places that corner at 0,0 then when you virtually flip the part in CAM that corner will be at 0,0 and you just have to make another program. This works as many times you need to flip the part provided you can clamp it.

Oh! of course! You answered your own question. Absolutely, adjust for the "flipped" OP. Your fine, go to it! Use the tolerances you know to be true on the first OP. Compensate for the "flip". I wish I had your problems! lol

Luck.

I see you checked for backlash by stating that your axis is returning to zero, but this doesn't necessarily let you know if there is backlash or not.

Being you say you're new to this, I suggest verifying backlash first. Then ensuring your vice is square. Then the above referencing replies can be used to properly reference the part. I can see where all of the above being out would start stacking movement error and creating the scenario you describe. Also be sure you zero the part the same way on both sides. As was mentioned a drilled hole works great as well as a stop on the vice and square it only using the fixed side jaw edge and either a parallel or 123 block.

You should also ensure the mill is properly trammed properly. I add issues in the beginning from the column being out while the has was still accurately square to the table. So check that as well.

Are you running backlash compensation? And also were your motors tuned properly for accurate movement taking backlash out of the equation? It's your first post so I am just throwing any circumstances out there that may be creating your issue.

That would include your complaints of poor surface finish that backlash certainly doesn't help.

Chris

Whilst I see a stop would work if the part is symmetrical and a mirrored G code programme is run, I also see the merit in a through hole / reference feature that can be zero'd again with a mirrored G code but for simplicity and providing no additional contouring etc. is required on the reverse, then the oversized block, single side machining with reverse side reduction facing has got to beat all for simplicity?

Quote:

---

Originally Posted by kawazuki

Whilst I see a stop would work if the part is symmetrical and a mirrored G code programme is run, I also see the merit in a through hole / reference feature that can be zero'd again with a mirrored G code but for simplicity and providing no additional contouring etc. is required on the reverse, then the oversized block, single side machining with reverse side reduction facing has got to beat all for simplicity?

---

I don't see how that's simpler if the OP already has a decent CAM. With a stop the part doesn't have to be symmetrical oe rhe stock doesn't all have to be exactly the same, since the second program is referenced on an already machined surface. What's more easier?

Thanks for the reply,
It’s the cnc side I’m new to, been working with manual machines for a while, trying to teach my self how to run a cnc mill so it can do one thing, while I work on others. The mill is trammed as best I can, the vice is indicated square, and I used a parallel against the solid jaw as a stop for the flip( start with a little rough stock past the outside of the jaw for the first run, use a stop on the finished edge when I flip.

Quote:

---

Originally Posted by TheSteelDragon

Thanks for the reply,
It’s the cnc side I’m new to, been working with manual machines for a while, trying to teach my self how to run a cnc mill so it can do one thing, while I work on others. The mill is trammed as best I can, the vice is indicated square, and I used a parallel against the solid jaw as a stop for the flip( start with a little rough stock past the outside of the jaw for the first run, use a stop on the finished edge when I flip.

---

Aye, but when you flip the part is not located as per the first operation since it was oversized to begin with. That's why to make it simple just make a new program in CAM with the finished edges referenced. You can't just run the same program. Otherwise you'll have to reindicate the part which to me is a waste of time. And you may not know the offset unless all your blanks are exactly the same size, which to me is also a waste of time to do (that's why we have CNCs!) So, you should have a physical stop on the SIDE of the jaw (even a small clamp holding some scrap plate would help) on the fixed side of the clamp, and call that theoretical corner 0,0. It doesn't matter which quadrant you work with in CAM.

There's a great video on this in the OneCNC site, but you have to be a user to access it. I have the video downloaded but it's about 30MB, maybe I can dropbox it...