ROLLDIE should be in your c-hook directory ALT-C. What version are you running?

There is another way to handle this part, which may be easier. Unroll the ID contour, and offset the walls by the cutter radius. Then cut that contour without offset, using axis substitution.

Look at HEAVY2.MC9. I created some centerlines and the toolpath. The sides of the wider slot won't be parallel, but that's OK, it's rotary clearance.

It looks like a pin goes in this slot. If it does, the walls should be parallel, and should not go thru the axis. Use rolldie with the slot option, and work from the centerline. You have to make the centerline, though. Unroll the inside diameter geometry, and work from that.

Use DRILL5AX and a cylinder surface. Since the surface is a cylinder, the output won't be 5-axis.

You can modify the post from the -.PST file all you want. I doubt you'll need a '2020' line in the -.NCI file. Explain what you're really trying to do, and people can help you.

If it's a rather small calculation, you can use the MP language (post language) to create points or lines, and output them in an ASCII file. SPROCKET.MPK is a good example. Find it in TEXT_&_POST_FILES_&_MISC on the forum. You can write a program that has no input, another ASCII file input, or a toolpath input.

It's not clear what you're making, or what kind of machine tool you have. Are you making a helical gear? Do you have a 5-axis mill? You should be able to program for the helix with a diagonal line, using axis substitution. I can add more when I understand the setup.

Millman: I don't fully understand your question, but here is the answer. MP makes a great stand-alone language. MP.DLL is the exec for all postprocessors. The -.PST file is a configuration file where you put all your code, so you are rarely conscious that the exec exists. You write a 'post' (xxx.pst), but have a dummy input (xxx.nci). The postblock PQ is accessed before anything is read from the -.NCI file, so do all your work from the PQ postblock. You can have inputs from prompts or the 'buffers' (xxx.TXT files).

This groove is tricky. The height of the rectangle in the flat is .587. The arc length of the groove on the OD (.9375 radius) is .597, and the arc length at the bottom of the groove (.8875 radius) is .565. The radius that gives the right arc length is .9217, or 1.8435 diameter. Use this diameter in the 'rotary axis' box in the toolpath prompt. The groove has sides that are radial (would project to the axis), so use ROLLDIE.DLL, and add .0342 to the depth (.9217 - .8875).

Look for SPROCKET.MPK in the TEXT_&_POST_FILES_&_MISC folder. After you unpack it, open SPROCKET.PST with an editor, just to read the instructions. The method of construction is right out of Machinery's Handbook. Let me know if you have trouble, or even if you don't.

Sometimes you can 'debug' a buffer by setting the 'keep' flag in the FBUF buffer declaration. Change the second parameter to 1. The 4 parameters are: buffer number, keep flag, no. of coordinates/record, read flag. The keep flag is 0 to discard, 1 to keep. The read flag is normally 0, 1 to read an existing buffer. The extension for buffer 1 is -.TX1, etc.

If the post can't read record 2, then the 2nd record in the buffer hasn't been filled yet. You can read any record in a buffer, but not past the end of the buffer. You must write to a buffer in ascending order, or you will get a similar message.

Have you tried plunge milling? There would be a lot less side force.

What post are you using? Posts based on MPGEN5AX should work OK. Random posts may not. Are you sure your post matches your machine?

It depends on the follower(s). If there is only one follower, still model the cam profile at the center of the follower, use ROLLDIE, and offset by the difference between cutter radius and follower radius. If there are TWO followers bracketing the cam 'key', I would have to know whether they twist, etc. Can you show more of the problem?

I'm going to side with the operators on this one. It shouldn't take 15 blocks to go one-half of a degree! This amount of data is choking the machine. Where did all that data come from? (What form was it in originally?). Could you make use of a cam generator?

Martin, Read my post. I made a 5-axis flowline toolpath to get a 3-axis curve with no offset whatever. I suppose I could have used a very small cutter, but this is cleaner. Then I stripped out the normals of the 5-axis -.NCI file to make the picture, using 5to3.pst. This gives me an ASCII -.NC3 file which is the blue lines. We still don't have the break between the straight lines and the fillet. I have posted a curvature analyzer curve.pst. That shows length (SUM), curvature (K), and radius ®for Q9.NCI. Notice the transition is not crisp between the flats and the radius. Neverless, CURVE1.PST and CURVE2.PST pick out a curve where the radius transitions a 2 inches. Backplot Q9.DOC with FILE-ASCII-CONVERT...

Martin, I have loaded 2 files to Text & Post files. One is 5to3.pst, and the other is Q9.NC3. Q9.NC3 is a 5-axis flowline without the normals, made from 5to3.pst. You could possibly luck out with flowlines made in the other direction, and pick out the two you want. Otherwise, you could pick out the break between a straight surface and the fillet surface from Q9.NC3 with a 'post' that would work on the line segments in this file.

Parts like this are good candidates for ROLLDIE.

I agree the quote was goofy. For a job that cheap, you should just turn a male screw and cast the threads with the screw as a mold. There's some pretty good compound made for just this task.

I go way back, so Create Line Endpoints is C-L-E.

Hi Mick, This is a 4-axis toolpath. Use ROLLDIE.DLL. Unroll the geometry and float an arc between the first and last points. UNROLL breaks data at each revolution, so you have to translate one end x-number of turns in Y. Use ROLLDIE on the UNROLLED arc, but you may have to BREAK INTO MANY. In general, variable pitches are best done in the flat with either an arc or SPLINE-BLEND. See VRAUGER.MC9 in Tech Support from Mastercam.

Hi Frank, I blew the last part of my reply -- TOOLPATH-PROJECT is a legacy (old) function, and really doesn't fit this problem. Use the c-hook FLOOR5AX. Make the 2d toolpath, then project it to the floor (hub) using FLOOR5AX. There's a peculiar bug in it. Select the OPERATION (OK the toolpath), select COMP SURFACES (the hub), select APPROACH/RETRACT (use the 3rd option, ...normals and vectors, THEN select AXIS LIMITS and OK - this fixes the bug, where axis limits aren't initialized unless you select it. On my second try, the blade thickness was .087.

Hi Frank, First, move whole part to top view, on center. Create a clean hub by CREATE-CURVE-PROJECT, projecting a straight line thru the origin on the surface. The cross section is a line and an arc. Extend the line .5 in. on the OD, and CREATE-SPLINE-CURVES with the line and arc to get a spline. Create a revolved surface with this line. Now you have a clean hub. The blades are 2 arcs, .090 apart. If you make new arcs, it will be easier to extend them. I think you can use a .250 cutter with a .0625 radius. Offset the arcs .125, and make a flat surface between them. If you do it right, it can be machined flowline. Then project the flowline toolpath to the hub TOOLPATH-NEXT MENU-PROJECT. This will put the toolpath right on the hub without moving anything in the top view. The fillets against the walls will blend into the hub, but I would leave them alone. If you machine one way towards the center, the cutter will cut cleaner, since it's moving upwards. Same method for roughing with a larger cutter. The little scrap of a fillet looks like it shouldn't be there. The left curve of the cavity needs to wrap around the tip of the blade a little bit before you create the flowline surface.