G53 command

mwinterm

In Wikipedia it states:

G53 Machine coordinate system : Takes absolute coordinates (X,Y,Z,A,B,C) with reference to machine zero rather than program zero. Can be helpful for tool changes. Nonmodal and absolute only. Subsequent blocks are interpreted as "back to G54" even if it is not explicitly programmed.

If tool length compensation would be considered this would not work for tool change (which is my problem).

https://smithy.com/cnc-reference-info/coordinate-system/machine-position-commands/page/0 also states: Regardless of any offsets that may be in effect, putting a G53 in a block of code tells the interpreter to go to the real or absolute axis positions commanded in the block.

Another reference on Youtube.

timcurtis67

@dc42 said in G53 command:

G53 does cause the WCS to be ignored, but not the tool offsets. Is there anything in the NIST standard or other documentation that says that G53 should cause tool offsets to be ignored too?

Yes G53 should only read true Machine zero's without any compensations. So you can return to certain positions for fixturing or tool changes. But it shouldn't cancel any compensations though.

dc42

Is there any requirement for G53 to be supported as a modifier for G2 and G3 arc moves? There is a specification problem with modifying G32 not to apply tool offsets, because of the the axis mapping that RRF supports which is predominantly for IDEX machines. I can get round that by defining G53 as making the move a raw move, so that no axis mapping takes place. But that doesn't make any sense for G2 and G3 moves. So I am considering making G2 and G3 abort if G53 is in effect. Is that OK?

Danal

This post is deleted!

Danal

@dc42 said in G53 command:

Is there any requirement for G53 to be support as a modifier for G2 and G3 arc moves?

The NIST standard explicitly states that G53 does NOT apply to G2 and G3 and so forth... Bolding mine:

3.5.12 Move in Absolute Coordinates — G53
For linear motion to a point expressed in absolute coordinates, program G1 G53 X… Y… Z… A… B… C… (or use G0 instead of G1), where all the axis words are optional, except that at least one must be used. The G0 or G1 is optional if it is the current motion mode.

It further states:
It is an error if:
• G53 is used without G0 or G1 being active,

Danal

Furthermore, in section 3.2.2 (definition of coordinate systems) we find the statement:

You can make straight moves in the absolute machine coordinate system by using G53 with either G0 or G1.

dc42

Great, thanks. I'll make G2 and G3 ignore G53.

Danal

@timcurtis67 said in G53 command:

@dc42 said in G53 command:

G53 does cause the WCS to be ignored, but not the tool offsets. Is there anything in the NIST standard or other documentation that says that G53 should cause tool offsets to be ignored too?

Yes G53 should only read true Machine zero's without any compensations. So you can return to certain positions for fixturing or tool changes. But it shouldn't cancel any compensations though.

Tool offsets ARE part of the concept of a "Control Point". Put Simply G53 internal calculations do include tool offsets.

NIST:

2.1.2.3 Controlled Point
The controlled point is the point whose position and rate of motion are controlled. When the tool length offset is zero (the default value), this is a point on the spindle axis (often called the gauge point) that is some fixed distance beyond the end of the spindle, usually near the end of a tool holder that fits into the spindle. The location of the controlled point can be moved out along the spindle axis by specifying some positive amount for the tool length offset

I believe Duet/RepRap is already behaving correctly here... but have not personally verified.

timcurtis67

@dc42 said in G53 command:

G53 does cause the WCS to be ignored, but not the tool offsets. Is there anything in the NIST standard or other documentation that says that G53 should cause tool offsets to be ignored too?

I personally have never used a G53 coordinate to do arc moves in my 30+ years of programming/operating CNC machines.

It's usually for moves to reference moves with G0's but could be used with G1's as well. I can't see any reason to use it for full motion tool paths.

mwinterm

Same here, G53 is only used to end up in certain hardware related positions for tool change, lubrication.... So no need for G2 and G3 and never seen so far that it works with G2 or G3.

@dc42 : Thank you very much for fixing this. Please let me know as soon as you have something on Github I can pull from.

Regards,
Marc

mwinterm

Tool offsets ARE part of the concept of a "Control Point". Put Simply G53 internal calculations do include tool offsets.

NIST:

2.1.2.3 Controlled Point
The controlled point is the point whose position and rate of motion are controlled. When the tool length offset is zero (the default value), this is a point on the spindle axis (often called the gauge point) that is some fixed distance beyond the end of the spindle, usually near the end of a tool holder that fits into the spindle. The location of the controlled point can be moved out along the spindle axis by specifying some positive amount for the tool length offset

I believe Duet/RepRap is already behaving correctly here... but have not personally verified.

I can't read it out of this that G53 should include tool offsets and neither on Heidenhain, nor on Sinumerik or Haas I have seen this being the case (for Haas you can check the youtube video I linked further up). It just would not work for tool change which is the most common use of G53 I'm aware of...

timcurtis67

@mwinterm said in G53 command:

Tool offsets ARE part of the concept of a "Control Point". Put Simply G53 internal calculations do include tool offsets.

NIST:

2.1.2.3 Controlled Point
The controlled point is the point whose position and rate of motion are controlled. When the tool length offset is zero (the default value), this is a point on the spindle axis (often called the gauge point) that is some fixed distance beyond the end of the spindle, usually near the end of a tool holder that fits into the spindle. The location of the controlled point can be moved out along the spindle axis by specifying some positive amount for the tool length offset

I believe Duet/RepRap is already behaving correctly here... but have not personally verified.

I can't read it out of this that G53 should include tool offsets and neither on Heidenhain, nor on Sinumerik or Haas I have seen this being the case (for Haas you can check the youtube video I linked further up). It just would not work for tool change which is the most common use of G53 I'm aware of...

The Fanuc and Mitsubishi controls do not add tool comp to G53 either. It's a true position of each axis based on the true machine home position without any tool comps.

Danal

@mwinterm Hmmm... I very strongly agree that G53 arguments are "machine coordinates", with absolutely no offsets of any kind. Nothing else makes sense to the operations that occur on real machines, as you've pointed out.

I also agree this is shown in the HAAS vid, right around 1:28.

The "Hmmm...." is because of the odd phrasing in the NIST standard. Let me poke around a bit more.

Danal

Well, I can't find anything in the standard. However, the standard is an attempt to describe the interpreter itself, and the interpreter is still available. Old, and in a very old "coding style"... but still out there.

Reading the old RS274NGC source, tool offsets are not applied when G53 is (non-modally) active.

As we all said...

mwinterm

@dc42: This post kind of also relates to the G0/G1 discussion I raised in another post (https://forum.duet3d.com/topic/7728/g0-vs-g1-movement). For the G53 to really function correctly for tool-changes etc. bed compensation also needs to be disabled for G53 G0... . I'm not aware if the standards say anything regarding G53 G1... but having G53 G0 ignoring all compensations (WCS, Tool & Bed) and having G53 G1 ignoring only WCS and Tool but keeping bed compensation in could give all the options.

dc42

Thanks to all of you for the references. I made a change ni 2.02RC5 so that tool offsets are not applied when G53 is active.

mwinterm

@dc42 Thanks a lot. Already built and tested it (even though not yet extensively) but everything seems to work fine

mwinterm

@dc42 : ...just noticed that there is already a built RC5 available... However I saw that in the release notes you refer to a modification of G54 instead of G53.... small typo but could be confusing as G54 (i.e. WCS) should for sure take tool offsets into account....

dc42

@mwinterm said in G53 command:

@dc42 : ...just noticed that there is already a built RC5 available... However I saw that in the release notes you refer to a modification of G54 instead of G53.... small typo but could be confusing as G54 (i.e. WCS) should for sure take tool offsets into account....

It should have read G53. I have corrected it.

mwinterm

@dc42 I detected another behavior of G53 which I believe is not correct. If G91 is selected G53 also makes relative moves which I believe is not correct. As outlined in earlier posts G53 is typically used to move to fixed machine position e.g. for tool change... This should happen independently of if G90 or G91 is selected.