Setting Work Cordinates

[Brad Cavallaro]

Hello, 

I have been working on this issue for about a week and can't seem to figure it out. I'm completing the First Part Tutorial.

My problem is that I keep getting the error "Linear move on line 41 exceed Y-Axis positive limit." I am assuming this is because the work coordinate location is not set correctly. What I don't understand is that when finding the edges, what is my starting location? Do I start at the machine home position, which I think is 0,0,0,0,0, or is it from the G54 location that is preset in the tooling page of the Pocket NC interface (-63.5, -63.5, -93.786, 0, 0) (XYZAB)? 

The page HERE describes how to set the work coordinates through edge finding, but it does not state from where eg, machine home, or from the work origin. 

Thanks for your help, I sincerely appreciate it! 

[gre...@gmail.com]

When you set up the job in CAM the co-ordinate system should be centered around the point on the b-axis about 21mm above the table (which lines up with the a-axis), the G54, that's all you need to do. You don't need to do anything on the machine except home it.

On your typical 3-axis CNC you would likely edge find the part and set work co-ordinates to the corner of the part say. On the pocketNC you can't do this, essentially the part must be correctly placed in CAD with respect to the G54 location. That page is really showing how to measure the position of the part wrt to that G54 origin so that you can tweak the CAD to match reality.

You can see where they adjust the offset from the origin in the CAD to match what was measured. For the part tutorial you don't need to be so accurate and positioning it as described will be fine.

Hopefully reading again with this in mind will make it clearer. 

Cheers,

Graham

[gre...@gmail.com]

I should add that when doing straight forward 2.5D or 3-axis work you can do work co-ordinates in the normal way, I've just never bothered myself as I am always doing 3+2 or 5-axis.

Graham

[qrot...@pocketnc.com]

Graham explained that well. To accurately use all 5 axes of the Pocket NC, the G54 work coordinate has to be set to the center of rotation (where the center of the B axis and A axis meet), which we refer to as the B-table offset. By default, this position is already set for G54. The values you see in the DRO after homing (except for Z) represent the distance each axis would have to go to get to that G54 location. 

As Graham also mentioned, the edge finding is simply to figure out where your already placed stock is in relation to that center of rotation. This way you can place your stock first then make the CAD/CAM match, as opposed to the opposite. 

Are you experiencing the Y axis limit error when A axis is at 90 or 0 degrees?

Thanks,

Q Rothing

Applications Engineer, Pocket NC

[Brad Cavallaro]

Hi Graham,

Thank you very much for your detailed response. The logic makes complete sense, however you say that " The part must be correctly placed in CAD with respect to the G54 location". With this logic, it is my understanding that I must measure the distance from G54 to material stock by jogging the machine first to the G54 location in the X and Y. However, I don't know the G54 location, and the edge finding tutorial does not say to start from the G54 position when measuring to the stock face. Thus,  is implied to start from the machine home position (0,0,0,0,0) and measure to the stock face. 

So if I must go to the G54 location, and measure to the stock face from there, how do I find the G54 location in X, Y and I think even Z?

Side note, I have also had the same error with Z being out of range. This indicates to me that I also have to set Z to G54 and set the DRO to 0 for Z, Y, Z, at the G54 location. 

Thanks again for your time and assistance! I appreciate it and am thoroughly enjoying the learning. 

[Brad Cavallaro]

Hi Q, 

Thank you for your additions, and thanks for the videos you've created, they are very helpful! In response to your statement "The values you see in the DRO after homing (except for Z) represent the distance each axis would have to go to get to that G54 location." Because I have messed with the DRO, thinking I needed to zero it out, I set the machine home to 0,0,0,0,0. If this is not correct and should reflect G54 location when homed,  how do I correct this? 

Also, I am experiencing the Y-axis limit when A is at 90 degrees. 

Brad Cavallaro 

[qrot...@pocketnc.com]

Hi Brad,

I know we spoke on the phone but I wanted to answer your last question here in case it might be helpful to others. To reset your G54 location to where it should be, you can navigate to the "Work Offsets" section of the Tooling page in the the Pocket NC user interface. From there you can click on the G54 icon and select "Remove all offsets". 

Best of luck! 

Q