Changing origin after toolpaths are created

[JPensack Acker Drill]

I made all of my toolpaths for a mill part and now i realized that I need to change my zero. What is the best way to move my origin and have my toolpaths not get messed up?

[veritasproject]

make a new wcs for the new zero and go to edit selected operations/edit common parameters then go to the planes and change it to the new wcs

then update your z depths in all your toolpaths

[gcode]

I'm assuming all your toolpaths are in TOP WCS

and TOP tool plane

1. Make a point where you want the new orign

be sure the Z value is correct..

Open the View Manager and make a copy of Top

and select yout new origin point.

then selact all you operations, right clcik and

use the "edit common parameter" to change

the WCS to the new WCS you created.

all your OPS will go dirty.. regen and you're done

[cobra95kev]

I try to use incremental as much as possible so all the ops will update fine in Z depth.

[Guest CNC Apps Guy 1]

quote:

---

I try to use incremental as much as possible so all the ops will update fine in Z depth.

---

+1,000,000 to that. I ALWAYS use incremental unless I absolutely positively cannot get away from it (which is fairly rare) for EXACTLY this reason.

[gcode]

Your Z depths should be fine incremental or absolute.

If the point your define your new WCS with has the

proper Z value.. all Z depths in your toolpaths

will still be correct..

That point is the new 0,0,0 and your toolpaths are defined from there.

[JPensack Acker Drill]

Thank You all for the replies, what gcode said was what I was thinking of doing but I wasn't sure how my toolpaths would react to the change. My Z will be the same so the z depths will be fine. Once again, Thanks.

[Colin Gilchrist]

Instead of copying Top, you can just go into the View Manager, click on the "Enable origin" button, then use the "select arrow" to go pick the new point.

 

That way you do not have to re-select a new WCS for your toolpath operations. They just update. Since you are not moving the Z origin height, your toolpaths will work as-is...

 

Edit: ok, I just realized that if you do choose to move the origin for the System Top view, it can give you problems with stock location in Verify. So do what the other guys recommended, otherwise you get unintended consequences...

 

Thanks,

[Superman]

If it isn't a plane change,

 

why not let the operator move the origin on the machine to suit your program by the same amount you wanted it moved.

[Jim at Gentex]

quote:

---

why not let the operator move the origin on the machine to suit your program by the same amount you wanted it moved.

---

Oh no you didn't just say that!

 

Many operators are still struggling with concepts like walking upright, and using indoor plumbing.

 

That, my friend, is a recipe for a crashed machine and / or a scrap part if I've ever seen one.

 

j/k

 

Seroiusly though, IMO the responsibility should rest on the programmer to make it as simple as possible for the operator.

[Superman]

quote:

---

Oh no you didn't just say that!

---

Jim

You don't tell your guys to set the origin 0.050" below the stock, or to the top of the fixture then add 0.250" for 1/4" plate-work

or

are you saying you've never done what I suggested

 

Boy, you don't give your operators any credit either ( I'd hate to be one of your guys, and read that post )

[Tim Johnson]

quote:

---

Jim

You don't tell your guys to set the origin 0.050" below the stock, or to the top of the fixture then add 0.250" for 1/4" plate-work

or

are you saying you've never done what I suggested

---

On most scrapped parts/machine crashes I hear the words "I assumed". I do everything in my power to take those words out of their excuses.