G51 scaling ??

If you have a question about the software please ask it here.

G51 scaling ??

Postby Vmax549 » Wed Oct 31, 2018 6:40 pm

Did I read correctly in teh manual that uccnc G51 ONLY scales from teh Work X0Y0 ?? AND you cannot set teh center of scaling to anything else ??

(;-) TP
Vmax549
 
Posts: 1380
Joined: Sun Nov 22, 2015 3:25 am
Location: USA

Re: G51 scaling ??

Postby cncdrive » Wed Oct 31, 2018 7:51 pm

Yes, just like with mach3. :) But ofcourse you can offset and scale from there.
However scaling and rotation are very buggy in mach3, I realised that when we developed scaling and rotation for the UCCNC and compared things with mach3...
cncdrive
Site Admin
 
Posts: 2301
Joined: Tue Aug 12, 2014 11:17 pm

Re: G51 scaling ??

Postby Vmax549 » Wed Oct 31, 2018 9:45 pm

Hi Balazs, Copying Mach3 is not always a good thing, :P . BUMMER :(

I am used to a G51 that sets up teh center of scaling and Scale factor. That makes it VERY easy to use.

G51 X1.111 Y2.222 I.5 J.5 where XY is teh center of scaling and teh IJ is teh scale factor.

The Mach3 method is almost without value. :cry:

Just Checking , (;-) TP
Vmax549
 
Posts: 1380
Joined: Sun Nov 22, 2015 3:25 am
Location: USA

Re: G51 scaling ??

Postby cncdrive » Sat Nov 03, 2018 2:02 am

Well, I get that Terry, but you know how it is ... if something works different as in mach3 then it is a problem and if it works the same then it is again a problem, so what should we do?!
cncdrive
Site Admin
 
Posts: 2301
Joined: Tue Aug 12, 2014 11:17 pm

Re: G51 scaling ??

Postby Vmax549 » Sat Nov 03, 2018 2:53 am

Best thing to do is look and see how the mainstream CNC controllers handle it. After all they have had DECADES to figure out how best to implement that function. Basically it should work similar to how G68 works . The center point can be assumed to be teh current position IF no XYZ values are declared. Then IF there are XYZ values declared then that should set the center of scale. THEN you can set teh scale value with teh IJK parameters X=I Y=J Z =K.

To do a simple 2.5d scaling it would be>
G51 X0Y0 I2J2

That scales everything from X0Y0 by a factor of 2.

A 3d object would be
G51 X0 Y0 Z-1 (bottom of part) I2 J2 K2

To scale an element say a carved emblem onto a door panel it would be
G51 X10 Y10 ( center point of element) I1.25 J1.25

It can also be handy to adjust teh dimensions of say a hole. Once teh machine cuts teh hole and you then measure teh hole. You find it is .002" off tolerance. You can simply go back set teh center point to teh center of teh hole and reset teh scale to adjust teh finish cut then rerun that section of code. Most of teh commercial probes support that function. It saves having to go back and recam teh entire project just to adjust the tolerance of a hole.

Another example is text engraving. Move to teh start of teh text. set teh centerpoint and scale teh text up or down. For example a consecutive S/N routine. Teh simple test is programed at 1" height. You then can simply scale it up or down Scale=1 then it is 1" scale =.375 the letter is .375" high Need it to be 1.25" high then set scale for 1.25

Scaling can be a very easy way to maintain teh aspect ratio of what you are working with.

Scaling can be very handy for things other than simply scaling up a simple 2D part.

One of teh worst case senarios in Gcode programming is to have to constantly shift offsets to do anything as it is VERY easy to make a simple mistake and then everything is ruined. By simply being able to define teh center of scale it is much easier than having to calculate what the offset should be then inputting it correctly.

THAT is one thing about old school programing I do not miss. Hopefully the general idea is to advance each function created as far into future as possible and still make it the most usefull solution .

Just a thought, TP
Vmax549
 
Posts: 1380
Joined: Sun Nov 22, 2015 3:25 am
Location: USA

Re: G51 scaling ??

Postby Robertspark » Sat Nov 03, 2018 7:44 am

Vmax549 wrote:
It can also be handy to adjust teh dimensions of say a hole. Once teh machine cuts teh hole and you then measure teh hole. You find it is .002" off tolerance. You can simply go back set teh center point to teh center of teh hole and reset teh scale to adjust teh finish cut then rerun that section of code. Most of teh commercial probes support that function. It saves having to go back and recam teh entire project just to adjust the tolerance of a hole.

Another example is text engraving. Move to teh start of teh text. set teh centerpoint and scale teh text up or down. For example a consecutive S/N routine. Teh simple test is programed at 1" height. You then can simply scale it up or down Scale=1 then it is 1" scale =.375 the letter is .375" high Need it to be 1.25" high then set scale for 1.25


I like those examples, can see a lot of benefit to g51 there
Rob
Einstein ― “If you can't explain it to a six year old, you don't understand it yourself”
...working my way through the 1000+ ways things don't work to find the one that does
UC400eth, UC300eth, UCCNC v1.2106, Neuron Lite
UCCNC v1.2105 Macro Manual
Robertspark
 
Posts: 1009
Joined: Sat Sep 03, 2016 4:27 pm
Location: Nr Liverpool, England


Return to Ask a question from support here

Who is online

Users browsing this forum: No registered users and 7 guests