Offset Question

[John H]

Hi All, I am sort of a novice at cnc vertical milling and I need some help in setting up a Haas vf-3ss Mill using a rotary table ,I am not sure the best way to hold the part and the correct way to set the offsets,My part is a rectangular alum block(1.5 x 5.375 x 7.125) and I want to face mill then machine a pocket in one side ,Rotate 90 deg face mill ,drill and tap a few holes,Rotate again 90 deg face mill(bottom) ,drill and tap,,rotate 90deg face mill(no drilling ).Not sure if a low profile four jaw chuck would work to hold it ,(semi production) on this part.Second question since the part is not square do I have to set new offsets for the different sides since they are diferent heights or do I use different work offsets,Can someone help me with this?

Thank You In Advance

[mishikwest]

Are you using a cam package or programing at the machine? For this type of part I use one offset and it is the center of rotation. For holding it maybe build yourself a little fixture? i.e. low-tech four jaw with set screws instead of jaws.

I've got one master subplate that is always on the 4th axis, and various fixture plates that bolt (and pin) on and off the master plate.

[John H]

mishikwest, Thank you for replying. I am using a cam software.So what you are saying is all my tool offsets are from center of rotation even tho the block is not a square block but rectangular in shape and I do not have to worry about the work offset? just use the center also? I am not the smartest person when it comes to figuring this type of problem out and I am grateful for your help.If you have anymore advis please feel free to tell me.


John

[keebler303]

if you set your offset to the center then you will set your depths as distance from the center, instead of depth.
if you look at the picture, the slots are both the same depth but are a different amount from the center. The distance from center is what dictates your position.
if one side of your block is 2 inches wider than the other, it will be 1 inch closer to the cutter. so to get the same depth cut you would go 1 inch less in depth than on the thinner side of the rectangle.

clear as mud?

Matt

[John H]

Matt, Thank you so much for that desription ,It has helped me to understand.If you have anymore advise please feel free to let me know.I will hopefuly be programing in mastercam,But right now Iam using partmaker.Again Thank you all for the help.

John

[mishikwest]

Let's say your using a hrt-210, then your z offset is 6" above the table. X and Y are simple edgefinder work. You will thus not need to change the offset for each side of the rotation. One offset for the whole part.

I program this way in Mastercam for this type of part. Then for each side just change the tool / construction plane for the respective opertaions, and my post processor will thus output A. moves.

[Geof]

You can also use G52 to move your offsets to the plane of the face you are working on. You set G54 to the centerline and the end of the block. Then if the first face you work on is 1.5inches above the centerline and the block is 2 inches wide and you want to use the nearest corner of this face for your work zero your G52 command is: G52 Y-1.0 Z1.5 Now the work zero that is being used is at the corner surface of the block.

When you index to another face you use another G52 command to move the work zero the the new surface and corner again.

At the end of the program you put in G52 Y0. Z0. and now you are back at the G54 location.

You do not have to put the G54 at the centerline for both the Y and Z, you only need to know where the location you want to use on each face of the block is compared to the position of G54. I often choose to put G54 Z at the top of the platen on the rotary with X at the front face and Y on the centerline. This position stays the same because the rotary always mounts in the same place. One advantage to having the work zero placed above the part like this is that the Z value for G52 is negative; if you make a typo and enter a positive number the tool just goes well above everything. When the correct value is positive and you make a mistake and enter a negative things get interesting when the tool tries to go way below where it should be.

[ctate2000]

First give very careful thought to the way you rotate your part. The description you gave could result in an out-of-square block. The easy way to program would be with one offset per tool and compensate in your program. Numerous offsets can bite you in the behind. Macro programming can be useful here. My opinion.