Need Help!- MastercamX3 and TM-1, G2 and G3 problems

[keithki]

Hello all,

I am just coming up to speed on both the machine and the program but I have one particular problem that shows up now and then. On three different parts, when I am creating a pocket with circular island, I am getting a different toolpath on the machine than I see on backplot, in all three cases plowing through the middle of the part. It seems like when I have a G2 or G3 command that is supposed to travel about 3/4's the way around a circular island with the island center as the center of the G2 or G3 command, the actual toolpath takes a shortcut, like in a counter clockwise circular path it goes straight from 12 o'clock to 3 o'clock, without going through 9 and 6 o'clock. I don't know if my Post is bad or there is a problem with the machine, or some kind of mismatch. I'm using MastercamX3.

Thanks, Keith

[Donkey Hotey]

You really should post this in the Mastercam forum instead of the Haas forum (you'll get more responses). I only have X so I can't say for sure but this looks to me like you may have lead-in, lead-out turned on and that may also be due to using Control cutter compensation.

Go back into your cutter path, change the compensation to either Computer or Off and turn off the lead-in, lead-out option. Post that and see how it runs in Graphics on the TM-1.

My guess is that if you really want to use compensation in the control (Haas), you'll need to do the lead-in, lead-out moves above the part, then ramp into the pockets. I haven't done this but I've seen the options in there.

[makingchips]

X3 is full of bugs. I had to go back to X2 MR2 SP1, Most of my problems were in live 5 axis programs.

Going back to X2 all my problems went away.


MC

[dcoupar]

It appears to me that the problem is in your post. For an arc over 180 degrees, R.2149 must be R-.2419

[Donkey Hotey]

Originally Posted by dcoupar It appears to me that the problem is in your post. For an arc over 180 degrees, R.2149 must be R-.2419

GAHHH!! I'm a moron. I didn't really make out what was going on in the pictures (and I was about to go to bed ). You're right, that is a different problem.

Note: the following is true for anybody using that generic Haas post in Mastercam. I don't know if they fixed it in subsequent versions but it's wrong in the one that shipped with X and probably X2.

If you want to globally alter that post & control definition (so this doesn't happen again):

1. Go into the Machine Type menu
2. Select Machine Definition Manager (doing it this way alters the master copy of the post, not the local one saved with the part)
3. Up on the icon bar for that dialog, you'll find a button for Edit The Control Definition
4. On the left side of the dialog, select Arc. This is where you set all the defaults for how Mastercam handles Arcs.
5. You should see a box that says Arc Center Type. If you want to use the 'Negative R' method, change that to Signed Radius. Do this for each of the tool planes.
6. Select the green checkmark (OK button) & saves all the changes

There are also options for IJK handling of arcs (Delta center to radius, etc) but I prefer negative radius (which it sounds like you want).

[keithki]

I think you are right on. Last night I stumbled across the control definition page and played with that very setting. In a quick test I found that "signed radius" solved the problem, but since I was in trial and error mode I wasn't really sure I had solved the problem or why. Thank you so much, this has been bugging me for a while. When you can't trust your silmulation and post it makes every program an adventure.

Thanks again, Keith

[Donkey Hotey]

You're welcome. I should add that it wasn't really altering the post file. By making that change, we altered the Control definition which is somehow different (I'm still trying to get my brain around the whole Mastercam post, machine, control definition thing).

Glad you got it fixed.