4th / multiaxis output

[pinguS]

Ok this is understandable.

Also when using the machine simulation, if you change something in the MAC file under 5 axis sim stuff, the changes can only be seen if you reload solidcam, is there not an easier way of telling it something has changed?

Another thing, i accidently changed the part to a 3 axis post in the coordinate settings. Now when I select my 5 axis post, the list box is greyed out and still says 3 axis, before it was 5 axis. Ca this be changed anywhere, or do I have to re machine the whole part again in solidcam, because now my machine simulation if throwing alot of positional errors due to rotation.

I don't mind even if I can go into the actual files directory and change something, so it reverts back to a 5 axis part???

[Brakeman Bob]

Also when using the machine simulation, if you change something in the MAC file under 5 axis sim stuff, the changes can only be seen if you reload solidcam, is there not an easier way of telling it something has changed?

Yes, just go into the CAM part setings (double-click the very top of the Job Tree) and reselect the MAC for the part, then recalculate all.

Another thing, i accidently changed the part to a 3 axis post in the coordinate settings. Now when I select my 5 axis post, the list box is greyed out and still says 3 axis, before it was 5 axis. Ca this be changed anywhere, or do I have to re machine the whole part again in solidcam, because now my machine simulation if throwing alot of positional errors due to rotation.

I don't mind even if I can go into the actual files directory and change something, so it reverts back to a 5 axis part???

No sure about this as I have done the same as you and when I reselected the five axis post and recalculated all, everything worked after.

By the way, one thing you can do to make things easier is to have a 3 axis GPP and a 5 axis GPP and just change the line in the MAC to point at which one you want to test.

[pinguS]

I've just tried the machine simulation

What the hell is this doing, I find that the simulation if rotating, like drilling around a block represents the drilling using specific axis. I.e. if I rotate a part in 90 deg so that I am drilling on the X+ face, I would assume it to show the drilling still in the Z dimention points, but this shows in the X dimention, as if I was doing a drill op in the X not Z.

Where do these come from. If I have rotated a part in 90 deg only on the Z axes, so that all I have done is just translated the X Y, nothing moves in the machine sim, but the post is showing the rotations. Does this work again totally differently to solidcam??

In the simulation, it only seems to rotate the part in the Z and X axis visually??

Also can the center of rotation when setting up the coordsys data be used in the post Gcode, I'm assuming you can use this to calculate the amount of movement to the next position when rotating (i.e. the depth of my B axis on the Y axis is 133mm from job Z face). I can't seem to find the variable to do so, if it exists....

[Brakeman Bob]

What the hell is this doing, I find that the simulation if rotating, like drilling around a block represents the drilling using specific axis. I.e. if I rotate a part in 90 deg so that I am drilling on the X+ face, I would assume it to show the drilling still in the Z dimention points, but this shows in the X dimention, as if I was doing a drill op in the X not Z.

Are you doing a drilling job using a different MAC to MAC 1 POS 1? When you use a different MAC position the axes are those defined in your MAC. If you are using the 5x_drill job option then I have no idea as I never use it.

Where do these come from. If I have rotated a part in 90 deg only on the Z axes, so that all I have done is just translated the X Y, nothing moves in the machine sim, but the post is showing the rotations. Does this work again totally differently to solidcam??

Look to your machine definition in the MAC file or the definition of your machine in the MachSim table. It sounds to me like either your order of precedence is wrong or you have a rotation about Z axis not enabled.

In the simulation, it only seems to rotate the part in the Z and X axis visually??

MachSim is not very illustrative of 2D operations - the move between one position and the next is not animated. Try to move the machine axes in manual mode of the simulator and see if your axes do what they are told. This will tell you if it is a post problem or a machine simulation problem. Get the machine movements in in MachSim right first, then move on to sorting out your post.

Also can the center of rotation when setting up the coordsys data be used in the post Gcode, I'm assuming you can use this to calculate the amount of movement to the next position when rotating (i.e. the depth of my B axis on the Y axis is 133mm from job Z face). I can't seem to find the variable to do so, if it exists....

The variables exist for X, Y & Z under "machine_offset_x" etc. and they pull the values held in the 3 boxes at the bottom of the MAC 1 POS 1 setting dialog called"Centre of Rotation based on Machine Co-ordinate System". It is important that these values are not in conflict with the machine base co-ordinates set in the machine definition.