[1320feet]

Personaly I never use offset finishing passes.

If you had to finish a bore that was to be .500 plus or minus .0002 with an end mill, how would one get there without offsets?

[Superman]

If you had to finish a bore that was to be .500 plus or minus .0002 with an end mill, how would one get there without offsets?

I'll talk Mastercam....
2 methods
1... geometry on-screen is your minimum size, cutter is defined to nominal diameter, tooloath type set to be "Computer" (no comp output), do a part cycle and measure size... you then modify geometry by how much you want it larger.
2... same as method 1, by you alter the tool diameter smaller by how much extra you want to cut.

.... criteria.... this wastes time and can lead to errors on creating a perfect path, any little error needs you to go back and alter the mastercam operation. You could do a tiny maths miscalculation and then ????

Ideally, you want 1 path that needs only having an offset change in the control.
Again... 2 methods, wear or control
1... Wear creates a path that when offset is set to zero, is already offset by ½ tool dia. Adjusting the offset positive moves tool away from your selected chain, negative moves it closer (onto) your chain.
2... Control gives a path that is on top of your chain, and the tool radius( or dia) needs to be placed into the offset. Any offset made larger than tool RAD makes the tool stay further away from your part. Smaller than tool RAD make it cut closer, making the tool edge to be over the chain.

Using Mastercam.... when chaining geometry to create a path, it is important to understand what the arrows mean when chaining. Big green arrow means the direction you want the tool to go, little green arrow is the side you want the tool to approach from (lead in/out needs to fit in the internal void, else it is omitted)
Where you pick on the 1st entity dictates start point and cut direction.
For a circle, the start point is 3 o'clock (0°), if you pick it at 12 o'clock will give large arrow going CCW, and small arrow pointing inward... this gives you a G41 output. This being for a bore.
If you pick at 6 o'clock the big arrow points CW, little arrow outward, approach is then from outside.... giving you a boss.
This is the natural method in creating toolpaths in Mastercam.
You are not limited to climbmilling everything, as long as you understand the meaning those arrows indicate. Set them wrong and the lead in/out is also wrong making you damage the part. You can change the cut side ( making G42 outputs) within the operation parameters.
Pick point at 6 o'clock (go CW), change side in parameters. will allow lead in & out to show on-screen.

[the_gentlegiant]

If you had to finish a bore that was to be .500 plus or minus .0002 with an end mill, how would one get there without offsets?

Ha... well let's start that I would not attempt that with an endmill to begin with. I'd bore or maybe ream it. Especially if there were any depth to the bore and you wanted to maintain decent circularity. But to answer your question.

I use offset toolpaths for roughing. All finish passes are created to the part or feature outline. Then comped to the radius of the tool and adjusted as needed. I do it that because to me it's easier, and the same toolpath can be used for finishing, chamfering, or switching to a different size cutter without re-doing the toolpath.

It would have made a lot of sense to let everyone know right from the git-go that offset toolpaths were being used. It's not a problem as tons of people do it. It may have produced better suggestions from those chipping in. I think a lot of people convert to offset toolpaths because they have a hard time managing the turning on and off of Cutter Comp. Case in point here with the origination of this thread. I do not suffer that problem so using offset paths never crosses my mind. It might be noted that I only program to 2d dxf type files. It's a rare occasion that I use a 3d part to program to, or do any surfacing. Mainly use form tools, and don't see a ton of that kind of work anyway.

Still interested in hearing when conventional milling gives you better finishes. :-)

[1320feet]

I'll talk Mastercam....
2 methods
1... geometry on-screen is your minimum size, cutter is defined to nominal diameter, tooloath type set to be "Computer" (no comp output), do a part cycle and measure size... you then modify geometry by how much you want it larger.
2... same as method 1, by you alter the tool diameter smaller by how much extra you want to cut.

This is how I use to do it. It was very time consuming when reloading large files into the Mori though a serial cable. So I now make the hole in Mastercam .001 to .002 smaller than I need. I then cut the first hole and measure. Then add to the radius offset in the fanuc control a positive number (as I'm using G42) to make hole larger to the size needed. an example would be to make hole in Mastercam .498 and cut. The hole after measured would be .4984. I would then add .0008 to the fanuc control to be on size.

Also, I have no problem chaining in Mastercam.

[1320feet]

Ha... well let's start that I would not attempt that with an endmill to begin with. I'd bore or maybe ream it. Especially if there were any depth to the bore and you wanted to maintain decent circularity.

To setup a boring bar is time consuming. To add a reamer to the tool changer also adds time. I almost always have a 1/8, 1/4, 3/8, 1/2, and a 3/4 endmill in the tool changer. So I grab one of those and bang out the holes needed. I usually only use g42 on dowel pin holes or bearing fits.

[1320feet]

Still interested in hearing when conventional milling gives you better finishes. :-)

98% of what I do is climb cut. I use G42 to make a bore larger with a positive number in the control is all.

[the_gentlegiant]

98% of what I do is climb cut. I use G42 to make a bore larger with a positive number in the control is all.

Sorry... I thought that was you who said something about fine finishes while conventional milling. I see now it was someone else.

I get what you're doing with G42 and an offset path. Got no problems with that.

So you're doing plus or minus 2 tenths day in and day out interpolating? Round holes? No bellmouth? No axis transition marks? Loading a reamer is too much time? Your work in a different world then I. Almost feel sorry for you.

How old and what Mori are you running? I have a 97 SV50 completely rebuilt. New rails, new screws, the works. I also use G8 Look ahead all the time. Have you ever tried G314 Quadrant Projection Compensation? Supposed to eliminate axis transition marks. I tried it only briefly. Curious if you've used it and/or mastered it's settings. It's on the last page of my Mori Programming Manual.