Is there a quick way to swap spindles in a pgm?

[woodturner]

Hello All,

I was wondering if there was a quick way to take an .sbp file that has been posted for one spindle, and change it to run the other spindle instead. In other words, automatically populate it with the offsets and on/off commands as if it had been posted using the 2nd spindle post.

Thanks in advance for any suggestions.

[Brady Watson]

Not easily.

Changing the on/off commands for the spindle is easy. Change SO,1,1 to SO,2,1 to turn on Spindle2 instead of Spindle1. (Off is SO,(output#),0)

Then you would have to make a little program for yourself that added your spindle offset for Spindle1 routines, and subtracted your offset values for Spindle2, depending on which SBP you wanted to change.

In short, if you wanted Spindle2 to do what Spindle1 was supposed to do, you'd have to 'cook' the code like this, assuming there is only an offset in X:

M3, X value (minus offset), Y value, Z value

I believe offsets for PRT tools are in the X axis & PRS tools are dominantly in the Y axis, do to the differences in hardware.

I would venture to guess that whatever you are cutting is much easier to re-draw, setup and toolpath than trying to cook the file with a program.

-B

[woodturner]

Thank you for responding Brady. In this case, it's probably easier to make a tool change. I have been working with the door program from Mike Richards and Bruce Clark, and it quickly puts out the cut files needed, but only for the primary spindle. There are three bits involved and three changes. If I could get all three cut files using a straight cutter to run in my second spindle, I'm down to one tool change. It was just a hopeful thought!

Thanks again.

[Brady Watson]

Well...If that is the case, then all you need to do is the following:

Run your C3 command, or zero XY as you normally do. Run the code for Spindle1.

When done, with original XY zero untouched, move the tool the required distance (your offset distance for Spindle2, so that it lines up with XY zero for Spindle1) and then zero the appropriate axis there. Then run the code for Spindle2, as if it were Spindle1.

You can always get back to 'Spindle1' zero position by moving exactly opposite of your offset distance and zero the appropriate axis there.

Do a replace of SO,1,1 with SO,2,1 to turn on Spindle2 instead of Spindle1. Then find the SO,1,0 at the end of the file and replace with SO,2,0 to turn it off.

Does this make sense?

-B

[Gary Campbell]

Ed...
You can use the SB MTC to do this by selecting the proper tool number. I will swap the heads and apply offsets for you.

Here is anoother way to get this done. Similar, but slightly different than Brady's
Add this to the beginning of the file:

VO,1,&my_head2Xoffset, &my_head2Yoffset (enter proper offset from my_vars file
J4,,,4,4 (or some other equal height that is safe)
VI,X,Y,A,Z
Start spindle.... SO,2,1 ?
Cut file

Dont forget to swap the axis back when done:
J4,,,4,4
VI,X,Y,Z,A
VO,0 (thats Vee Oh, zero)

Read up on these commands in the programming handbook

[woodturner]

Thanks for both of the suggestions. Brady, I can easily get my head around your method with one exception. Does simply replacing SO,1,1 with SO,2,1 mean that spindle #2 now reads the "Z" changes to actually do the cutting?

This also means each tool path has to be "babysat." I was hoping to include the changes in the files and them make 2 master files (one before the tool change and one after). When nesting 20 plus drawer fronts there would be enough time to work on something else during a three file run.

Gary, my machine is a 4 year old +/- Alpha and I don't know if I have the command you are referring to. I am less familiar with what you're suggesting. Could you say if it would allow for the master program approach?

Thanks in advance!

[Brady Watson]

SO,2,1 = Set Output, 2, (1) ON

It just turns on an output switch that switches your VFD.

Gary's method will work if you upgrade your SB3 to a newer version.

-B

[Gary Campbell]

Ed...
Brady is right, my method will only work with the 3.6.xx (newer) software versions. Assuming that you are using one of those versions, and also assuming that you can assign a tool number to each tool, the MTC may be the best way to go. It will be a rather seemless approach, assuming the tool numbers.

An ol woodworking fart named Roger that used to hang around here has the perfect setup for the dual Z PRT. Maybe he will show up. As Brady can attest, my knowledge is only of the new machines and software.

Thanks for the catch Brady!

[Brady Watson]

...As Brady can attest, my knowledge is only of the new machines and software. Thanks for the catch Brady!

Gary,
Your modesty is hanging out again :D

Don't be fooled...Gary knows prenty :D

-B

[woodturner]

Thanks again. I will look a bit more into what Gary is suggesting.

Brady, I understand the SO, 2,1 will turn on the second spindle. What I don't get is what effect does that have on which spindle physically drops in "Z" into the panel.

In general the post processors are a mystery to me. Like my air drill post, "sometimes she feels like a nut, sometimes she don't."

[Gary Campbell]

Ed...
Take a look at my article on the "virtual toolchanger" It may help you get a grasp on what you want to happen, how it happens and how to make it happen. Link: http://www.shopbotblog.com/index.php/2009/06/the-shopbot-%e2%80%9cvirtual%e2%80%9d-toolchanger-part-2/

The only requirement is that you have a specific and unique tool number for each bit. The files that do this are included with the SB3 download and have full tech support. They use the variables that are already on your machine and will allow you to use any and all of your cutting heads in a single cutting file. (Vectric or Delcam software)

I am not sure the free doors program has full support. but those guys have their stuff together, so I guess you should be able to cut as you wish.