Page 1 of 1

XY Datum Offset

Posted: Wed Mar 20, 2019 9:30 am
by mezalick
Greeting All,
I'm just going thru a few items in the software and I realized I've never used the XY Datum Offset....Imagine that.....
So it got me thinking about when and why to use it......
I came up empty..
So my question is, when is it appropriate to use the XY Datum Offset..
I'm sure there are plenty of good reasons otherwise it wouldn't be included in the software..

Looking forward to your ideas.
Thanks in advance.
Michael

Re: XY Datum Offset

Posted: Wed Mar 20, 2019 1:49 pm
by TReischl
One that comes to mind is that a part you are going to cut already has a hole cut in it. You want to use that hole to set the zero of the program.

Another is that you have a fixture that has a datum hole in it that you use for zero.

I dunno though, in about 12 years of using this software I have never found I needed to use it. ::::shrug:::::

Edit: On the mini mill I have an edge finder that I use quite often to find the center of a hole and then I use that to perform other operations after setting the DRO's. But on the router the spindle is way too fast to use that tool.

Re: XY Datum Offset

Posted: Wed Mar 20, 2019 2:42 pm
by Leo
I don't use it either - BUT

It would be a good point to have a "park" position away from the XY zero point so I can load/unload the part with the spindle out of the way.

I often just edit the G-Code to do that for me.

Re: XY Datum Offset

Posted: Wed Mar 20, 2019 3:05 pm
by ger21
I use it with our Morbidelli, which has a backwards Y axis from standard.
I set the Y offset to -49, and make the stock 49" high. This puts zero in the back with negative Y values in the front. I invert the Y values to positive in the post.

EDIT:

While double checking this, I realized that I can get the same thing by selecting back left for the origin and disabling the offset. :shock:
Lots of different ways to do the same thing. :)

Re: XY Datum Offset

Posted: Wed Mar 20, 2019 5:43 pm
by adze_cnc
You need to fool the software into believing you have a larger piece of material than you actually have so it will calculate finishing paths properly? viewtopic.php?f=2&t=31634&p=228815#p228815

I don't often use it but it does come in handy when it is needed.

Re: XY Datum Offset

Posted: Wed Mar 20, 2019 6:56 pm
by mezalick
Thanks Gents..

Steven,
It was your post that I saw that started me on this issue...Thanks for posting it.
Ger21,
Three options for everything I always say..LOL
Leo,
You can park the router by setting the "Home / Start Position" in the material setup window on the toolpath side,,if your PP is setup for it.
TReischl,
That's a good example, thanks


Michael

Re: XY Datum Offset

Posted: Wed Mar 20, 2019 9:44 pm
by IslaWW
I only use offsets in one way... To provide an intuitive drawing field when designing for my SideWinder CNC Wood lathes.
Setup.JPG

Re: XY Datum Offset

Posted: Wed Mar 20, 2019 10:39 pm
by mezalick
Make Sense Gary,,,,Thanks
~M

Re: XY Datum Offset

Posted: Thu Mar 21, 2019 11:47 am
by 4DThinker
I almost alway use it. I set X and Y value to 1/2 the diameter of the bit I'll be using first. Either may need to be a negative value depending on which corner I've chose. What it makes easy is zeroing X and Y by sneaking the bit up to the relative edge of the board until a piece of paper is trapped against the edge by the bit. I'll jog close, then use a .005" step which is also how thick paper often is. I find this much more accurate than trying to zero a bit on the center of a board. You would be surprised by how much off my students can be when asked to mark the center of their boards. When I'm starting a job with a V-bit then I skip the offset and just use the corner. I visually align the tip of the bit with the board corner.

4D

Re: XY Datum Offset

Posted: Sat Mar 23, 2019 5:59 am
by KeithW
When I'm starting a job with a V-bit then I skip the offset and just use the corner. I visually align the tip of the bit with the board corner.
I'll do this for any bit. If I need to zero off on the corner or the center, I just slip a v-bit in and center, then put in the bit I'm using and then set the z height. Seems to work as good a any...

Re: XY Datum Offset

Posted: Sat Mar 23, 2019 8:54 pm
by rscrawford
When Iā€™m using the cnc to cut on a lathe or an indexer, I want the xy datum to be in the centre of my material set up in the x axis but at the bottom in the y axis. So I choose the xy datum for the bottom left and then offset it half my material width.

Re: XY Datum Offset

Posted: Thu Mar 28, 2019 4:57 pm
by Will Williamson
A lot of times, when I get dxf file, from a new client, the file, will import, with that box checked.
If you are not careful, you will over look that check box.
You will soon learn about that offset.

Re: XY Datum Offset

Posted: Sat Jan 02, 2021 11:05 am
by badgersurfer
4DThinker wrote: ā†‘
Thu Mar 21, 2019 11:47 am
I almost alway use it. I set X and Y value to 1/2 the diameter of the bit I'll be using first. Either may need to be a negative value depending on which corner I've chose. What it makes easy is zeroing X and Y by sneaking the bit up to the relative edge of the board until a piece of paper is trapped against the edge by the bit. I'll jog close, then use a .005" step which is also how thick paper often is. I find this much more accurate than trying to zero a bit on the center of a board. You would be surprised by how much off my students can be when asked to mark the center of their boards. When I'm starting a job with a V-bit then I skip the offset and just use the corner. I visually align the tip of the bit with the board corner.

4D
I often wondered what this is for. So correct me if I am wrong. If I am using a 3mm bit and want to set my tool at the x=0,y=0 point (bottom left corner) of my material. I touch the tool on the x0 then on the y0 and set the offset to x=1.5mm,y=1.5mm to get the tool centre smack on the corner. Have I got the right end of the stick?

Re: XY Datum Offset

Posted: Sat Jan 02, 2021 2:17 pm
by 4DThinker
badgersurfer wrote: ā†‘
Sat Jan 02, 2021 11:05 am
I often wondered what this is for. So correct me if I am wrong. If I am using a 3mm bit and want to set my tool at the x=0,y=0 point (bottom left corner) of my material. I touch the tool on the x0 then on the y0 and set the offset to x=1.5mm,y=1.5mm to get the tool centre smack on the corner. Have I got the right end of the stick?
Yep. That is unless you're holding the left end of that stick. ;)

Re: XY Datum Offset

Posted: Sat Jan 02, 2021 2:48 pm
by nicksilva
here is an example - but it would only pertain to a production run. If you have a design you're cutting - say it has a critical drill hole and profile. You find the hole is .002" from where it should be in the Y axis. You would simply offset the Y axis that much so that it moves into the correct position for the next part. On a production mill such as HAAS (or Fanuc or Mach3/4), you can do it on the fly. But on hobby machines you can't so it is just as well to move the actual start point X or Y (G54) by the correct amount or do the datum offset in the software and redownload. The important thing here is you don't have to touch your design to fix the problem.