Need Help!- Is it possible cut with 4th axis tipped on 10 degrees?

[mfpuller]

This is related to my earlier post about the impeller, but I wanted to simplify my question. Is it possible to use a multlsurface toolpath with 4th axis output and a generic haas 4th axis post, cutting a around an "A" axis that is tipped up 10 degrees on a vertical mill? Hopefully sombedody has tried this or understands what I am asking. I am getting "A" codes that are approximately off 8 degrees. Thank you for any help you can provide.

[TXFred]

I haven't tried this myself, but my feeling is that the answer is yes.

[WallyL7]

I can't really answer in regards to the generic post or how your WCS is set up, but yes... it can be done - and quite easily.

Hopefully what txfred posted helps, or you may just need to have someone look at all your parameters in mastercam to make sure all of the correct protocol is in place. It's been a while since I've done it but I used to make Porsche pulleys that required what you are asking and it wasn't a huge deal to get right.

You may have to attach the file and have someone here have a look-see.

[Saint Mark]

Hi mfpuller,
I understand what you are doing, I do it almost every day on a 5 axis haas VF mill. In my case I fix the tilt axis and run multi surface 4 axis tool paths around the rotary axis. So to be fair it's the same in principle. My only main difference is I don't use mastercam posts. I export all my data as NCI files and then us a Campete product to post and collision check my toolpaths. Just for your info I only use the advanced multi axis toolpath options as these give me the best results and lots of control. Check out the tilt option on the 4th axis tab. You will need to input +\- 10 degrees depending which way you rotary is tilted.
With regard to your 8 degree error, I have never had issues with mastercam giving me inaccurate data and therefore feel this is not a prepost issue which leaves machine and tool setup (difficult to comment on this), the machine axis sync, I have experienced issues with this on the version 17 software, in this case some parameters were incorrect by the factory. A simple sphere chasing program with eliminate this. And lastly the generic post, as I mentioned earlier I don't use them. Maybe you could create a simple program that allows easy reading of a posted program, a square profile maybe, you could then cofirm the post is giving good data with a bit of trig.

I hope this helps, but what you are trying to do is possible.

[mfpuller]

I tried it again the other night, and I did get it to work. I had previously tried changing the machine definition tilt but that didn't work like you would think. I ended up programming and posting with generic 5 axis post, and it worked. I had tried this before but was having trouble keeping 5th axis locked, it would always move about .1 or .2 degrees. Just got back on here and read replies, and I was doing exactly what Saint Mark stated. The program I ran was just one side of one blade the other night, just to check post. Now that I am past post problem, the only problem I am still struggling with is keeping 5th asxis locked on the other wall paths. I have come to figure out that it is the gouge check that causes the post to make 5th axis moves. I created one surface all around the blade, but haven't had a chance to get back to programming this to see if this will help the situation. I think it's just of matter of smoothing toolpath, (easier said than done with this software it seems).