Need Help!- changing part setup for multiple ops

[Captdave]

Hi Guys,

I need a little advise on programming multiple operation on several sides of the same part. Pretty basic stuff but the jobs I have been doing so far haven't required it so my first go at it. So far I think I have figured out how to use the comment page to stop the program and tell the operator how to position the part for the next op and change setup page to define the new part XY0 for the current side of the part. But this has me puzzled, copied from the WinMax manual:

The Change Part Setup fields are defined as follows:
Offset Z—Defines the Z dimension offset for part zero. This field is usually left at 0 and the Tool Calibration field in Tool Setup is used to determine each tool's part zero. Does this mean that there are 2 offsets registered for the tool?

What I haven't figured out is how to change the graphics to show the current side being machined or if it is even possible. Seems like a basic need to be able to rotate the part and see the operations being performed on each side to verify proper programming. Do you make a separate program for each side? On Mazaks lathes, when the part needs to be turned around for second ops, its best to build a separate program and tell the control to call the next program which brings all the tool and offset info with it.

Please share and tips or tricks you may do to make this as simple as possible.

[glovebox20]

Hello

The easiest way I've found out out to do this Conversationally, Is to use "Change Part Set up" blocks in the "Misc." function.

Tool Touch off

The First thing you should do, especially if your going to use the same tool for multiple Op's, is decide a common Reference point to touch off All Tools. Whether if it's on top if a 2X4X6 block on the bed of the machine, or top of a vise jaw somewhere. It doesn't really matter as long every tool can reach that point and that point never changes.

On thing I will add is you might want to adjust one of your parameter under program parameters page so no matter what the Z offset is at in you part set up, It will always store the value from machine Zero and not Machine Zero plus Z offset in part set up. This will help prevent tool setting mistakes.

Pick up part zero

There are a few way you can program this, but the way I choose to do it is by leaving the Tool Set (under input screen) at zero. Then the first block in the program should be a (change part set up). While in this "Block" you should notice that you can manual jog the machine around. Pick up your X,Y,Z zero. To pick up Z zero, you can take a calibrated tool and touch it off on the part. what ever value it gives you, enter in your Z offset. Or you take a indicator and zero it out where you touch your tools off, then jog over to your part zero and zero the indicator out and enter the difference in your part set up.

Every Time you change to a different part setup, you will need a "change part set up" block. For this reason, it's easiest to do every thing in the one set first, than move to the next set up. Although if cycle time is important, you could program it to do one tool, all set ups, but this gets a bit tricky cause if you have 5 part set up for the same part and you need to adjust it, you need to change 5 part setup blocks. There is something called "transform plane" which are used with Rotary blocks, but I'd rater not get in to that right now, Unless you have a Rotary axis you can program.

Graphics

The Graphics will look different that you are use to. Instead of showing you part Zero On the Upper left corner of the part (for example). Part zero will be however many inches off the part according to your part set up. You can go to the part setup page under the input screen and make sure that part setup matches the current set your programing so you can view it right. Or it might be easier to use Graphics on/off "blocks" to show certain parts of your program.

On 4 or 5 axis Hurco mills, there is an additional field in the part setup called B distance Center line, Z distance center line, etc. All their for is to let you Tell the machine where the center of rotation is in reference of you part set up so the Graphics screen can draw it correctly. I'm assuming all you have is a 3 axis mill and this will not apply to you. You should see however is 3 (or however many diff. setups you have) spread across the graphics screen, according to your part setups. So if the center of part one is at X13, Y10 in your part setup, It should show you that your center of your part is at X13, Y10 on the screen. However, if you have a value in the part set under the input screen, this will affect this. It will not show the part rotated to a new face unless if you programed a Rotary axis (Rotary position blocks).



If your only doing one OP a time, It will be easier to have one program for each OP. But if your doing all the OP's at once, you probably want to combine them into one program.

If your still have troubles with this. I may be able to take your program, look at it, make some change/suggestions and send it back. Just don't expect quick turn around times.


Good luck

[Captdave]

All good advise. I used the desktop software I downloaded to try how you recommended to use part change set up and turning the graphics on/off it works good. I'll have to spend a little more time refining it but I think it will do what I'm looking for. For this job I think I'll just do separate programs for each op and run them individually for now.

I'm sure that there will be future jobs where this will work nicely.

Thanks for your input.

[glovebox20]

Thanks for the update

glovebox20