Printable View
Hello All,
I am trying to figure what plane to use for machining a part with 45 degrees chamfer.
But whatever I change the plane I always get this
G0 G54 G90 X0. Y0. C90. B-45. S3500 M3
C90 AND B-45. OK with B-45 but c i think it shouldnt change.
But any plane i change the GNOMON i get the same.
Any clues
Thank you
We need more information. Are you on a 5 Axis machine? Version of Mastercam? Can you Share the part file or at least a picture or print? Do you want to cut your 45 degree face normal to the face "side cutting" or face cutting with the end of the endmill?
Yes the machine is 5axis MAXIMA from cms with Fanuc 18i-mb5 control.Mastercam 2018. (I had the same problem with x9). I want face cutting with the end of endmill.
Please find ttached 3 files, mastercam toolpath. nci and nc.
Can you post your file as 2017 mastercam? I'm still on that. If not export it as a parasolid and make a screen shot with where you are setup and I"ll program it in 2017 so you can see how it's done. thanks
Thanks for your help,
please find the file attched as 2017 mastercam. Please note setup is different as my original 2018.
You need to create two planes. I named the main plane 5 AXIS START. You need to set your first planes WCS to what every point you want to setup off of. Next you need to create a plane facing the chamfer you want to machine. This plane I named 5 AXIS CHAM. You must set the new planes WCS to the same WCS point of the base plane (5 AXIS START). Now set the = to your base plane and then set your C plane and T plane to the second plane 5 AXIS CHAM. Once you do that set your view to the tool plane. Now you can program the chamfer surface like any 3 axis plane but when it posts it will be in 5 Axis.
Attachment 365100
Many many thanks, I will review and I get back to you.
Just a quick question. doesnt have the new planes to have the same origin as wcs? (origin is bottom right corner) planes seems to be on the center.
Yeah I just started over with your file. It doesn't matter where you setup your WCS, as long as your secondary plane is set at the same WCS point as your base plane. It could be the corner if you want just set them both the same.
I think I know exactly what you are asking. I've struggled with this for a bit in the two different CAM systems I use. I believe the origin for your "tilt" planes (T/C) makes no difference in the posted code. The post will look at your machine's axis combinations and choose the correct tilt combo (B and C in your case) and all the calculations will come from the WCS origin using the T/C plane as a reference. That is the short (and not quite accurate) answer I've discovered.Quote:
Originally Posted by platonas1
The way you set your T/C plane origins DO have an effect on your Z depths in the toolpath dialogs that use that T/C plane. For example, if the origin of the T/C plane in the pictures above was actually on that angled surface, the Z cut depth in the Linking Parameters page (in absolute) would be zero. If the origin of the T/C plane was at the WCS, the Z depth (in absolute) is going to be some positive distance.
There also may be some consequences of the rotation (about Z) of your T/C plane. I haven't experimented as much with this but in general I make sure I rotate the T/C plane to what I think is the "correct" rotation. The machine's axis combinations might come in to play here, I'm no sure.
He is using the wrong post kinematics of the machine. this is a A and C axis. Is this machine a Head < Head setup? as setting up the angle in 3+2 for this is easy. but if you are running the wrong machine def and post it may output different for sure. With a solid as show in you sample picking the gnomon and the face will set the Z in one click. you may need to swing the X or Y based on the machine kinematics.