axis limits

[Cbgstyles]

hi any body know how to set up axis limits , when I run a tool path it will error  , I've tried setting  machine definition and it does nothing

[Guest]

Not going to work...

 

No way to do as you ask that I am aware of..

[jlw™]

I have templates in which i have my fixture solids or vise models and a model of the table with an outline where i can run. Then I stay in it.

[JAMMAN]

I know some axis limits works on my DMG, on the tilt axis with my post and blade expert. I limit it to 90  and if I don't limit it it will go farther.

 

I can't see it working on XYZ due to work offsets, tool offsets and 5 axis positioning routines because XYZ could be anywhere depending on where your tables or head is.

 

But in case you are talking about your tilt or rotary you should be able to limit them.

[Colin Gilchrist]

When users talk about Travel Limits, many times they are referring to the Linear Travel Limits of the machine. By default, none of the 3X or 4X posts are setup to respect Linear Limits. In fact, even the 5X post does not track the Work Envelope of your machine. The 5X post only supports Rotary Travel Limits.

 

Machine Simulation can be setup to detect the Linear Limits, if you record actual "real" register offset numbers from your Control, and are accurate about where on the table you locate the part and fixture. You want to setup Mastercam so that the numbers in your CAM system match the real numbers on the machine.

 

Personally, I setup some logic in my posts to warn me when I'm within .5 of a Linear Limit. To do that, and have it work, you need to tell the post what the mathematical limits are, and also pass the data of where the Work Offset Origin is, in relation to Machine Home. I setup my posts to read the Home Position Values that I enter, and calculate the available travel in each axis direction. For example, if you're setting up a part on the far left side of your table, on a 3X VMC with 40 inches of X Travel, then your G54 X register might beven set to a number like X-36.2433.

 

That means that with an X Register value so far from machine home, you only have a minus travel range of X-3.7567.

 

MP will calculate the travel envelope of each Tool Path, giving you the Min/Max extents of each path. It's a simple matter to compare the Axis Values, and warn you that an over travel condition is present.

 

Most machines I've worked with over the years have Machine travels in the negative range. Typically, when the machine goes home, the spindle face, and tool axis centerline is the X0Y0Z0 position. When you jog the machine, the machine coordinates show the Axes moving in the negative direction.

 

On a Haas Mill, if you have travels of 40 x 20 x 20, for the work envelope, in reality the X Axis range is from 0 to -40, the Y range is 0 to -20, and the Z range is 0 to -20. So generally, the machine motion is on the minus side of machine home origin. On most machines, there is also an offset in the travel range of one or more axes.

 

What do I mean by an "offset"? Take the Z Axis for example, on the VMC I just mentioned. The last machine I checked had 4.25" of offset from the face of the Spindle Nose, to the machine table. So the travel range, measured from the table surface would actually be 4.25 to 24.25 away from the table. But the machine still treats the home position as the reference. So when you read the Machine Z Coordinates, the range is still from 0 to -20. (That "Machine Z Coordinate" of Z-20, puts the spindle face 4.25 inches above the table. If you want to track the Linear Limits, these details matter...