Need Lathe assistance ASAP please

Alright, I am programming a Nakamoura Mill turn. I am programming a turbine pump and shroud in Mastercam. So basically the shroud fits inside turbine blades. It looks very similar to this https://d2t1xqejof9utc.cloudfront.ne...3d0/medium.jpg

So only focus on the far left on the part. The blades on my part look similar but they are only x,z blades there is no contouring on the blade. now imagine a shroud that fits perfectly inside the blades. The contour of the blades SHOULD match the contour of the shroud perfectly.

There is a good size gap between the blades and the shroud when I try to match them up. This is where I think I made my mistake. I didn't use cutter comp at all in mastercam. I turned it completely off in mastercam and on my control I had my cutter geometry set to 0 for both height and diameter. I basically programmed it as if I were programming from a tool point. I believe this may have really messed up my contours. It looks like any where between .1 and .03 gap on a part that I have a mating tolerance of .005. Please help me out. Is my issue that I didn't use cutter comp? If so how do I set it up in mastercam lathe? Thanks!

btw this is x5 and the nakamoura is a fanuc control.

So what I did was program a part to the dimensions on the sheet and did not use TNR compensation. Should I set it to wear or in computer? The diameters appear correct but the actual contour isn't mathing up.

Edit, i just noticed this is for lathe.

Yes, wear or computer will work fine for a turning tool, you need to use comp or the radiuses get messed up, as do tapers.

Make sure in your control to set the value of the tool nose radius. Make sure the insert youve selected on your tool in mastercam is the proper radius that youre going to actually cut with.

I see in mastercam where to input my tool nose radius buy why do I need to add it in the fanuc control? and if so where is this done? I am guessing on the tool data screen so I will figure that out. If however I do comp in computer and the tool path is adjusted accordingly, why would I need anything in the control. I should just be able to leave the tool radius a 0 in the control? Thanks for the help so far!

bump

Yes you would inout it on the tool geometry page, there is a column for nose radius.

Reason for this is because thr tool is touched off in x and z, this is actually a theoretical point that is actually not on the tool surface at all. It will cut diameters and faces at the right points, but tapers and radiuses contact the tool differently, therfore thr tool must be compensated to keep it in touch wih the right point of the tool.

Basically the proper contact point is dynamically changing as the tool moves around the radius, so the control needs to know where exactly the actual cutting edge is to cut it properly.

Okay so input the tnr on the nc at the machine and inside mastercam when setting up tool parameters. Do I do cutter comp in computer or control or do I use wear?

I always thought if mastercam knows which insert you are using (in the edit tool), and you use wear as comp, then mastercam compensates for the radius. So I don't think you need to put anything in the tnr offset, if you use wear in mastercam.

Quote:

---

Originally Posted by utengineer04

I always thought if mastercam knows which insert you are using (in the edit tool), and you use wear as comp, then mastercam compensates for the radius. So I don't think you need to put anything in the tnr offset, if you use wear in mastercam.

---

I am pretty sure that is correct and that is what I did wrong. I am testing to today to verify. I will let you know how it plays out!

Everything came out in tolerance after the changes! Thanks a lot guys.

from my lathe programming days, i always programmed to control comp with zero tool nose radius. the set up guy inserts the TNR in the machine control. this way the machinist is not tied down to one sized radius and has more control at the machine end. this way G41 & G42 are still being generated.