I have a very major issue with Easel and I have asked this before and did not get a satisfactory answer.
Why, I mean really, why does Easel drop the z (you) to what ever the ‘safe’ height is before moving the X and Y???
Go to any machine shop that has CNC mills and see how they address this.
Always move to the X and Y coordinates before dropping the Z (tool).
Always, this is because of obstacles in the path (clamps, features, etc), this is so one does not break off tools before making a chip.
I do not use Easel to do any machining, I use it to design, this is because I have to edit the G code to ‘fix’ the errors in rapid moves.
Tedious at the least and a simple thing to fix in Easel code writing.
Come on guys, I do not know who is responsible for this but please urge them to vist a real shop where code is written and see what moves where and why.
It’s called safety height for a reason.
Sometimes you gotta work with what you got.
Remember also that some people go from setting the Z zero straight into carving so it needs to set the bit to SOME level and that’s why there’s a safety height.
From what I can tell you want the “Safe Height” to be higher? so that it doesn’t drop before it gets to the “work” area? that is a setting you can change. If you know the height of all your obstructions then set the “safe height” to that parameter. You might not have gotten a satisfactory answer as you are not offering a specific solution. The program is written to perform to most users needs and is customizable for users with specific needs (i.e. different step-over settings, different safety height, rapid movements etc.) and it is up to the user to change these to suit their specific needs. for most if it works then don’t mess with it. for those of use that it needs to be different then change it to suit your needs. If you can not change it then try something that works for you, as you stated you design in one program then change the code to finish in another. so if that work flow fits your specific needs use it. Before I get all the it won’t change until I voice my problems remember if you have a problem that only you have then why should everyone else change to make your specific and unique problem theirs.
P.S. I am all for using whatever programs work best for a situation as no one program fits all needs.
In easel
Machine > advanced
Box labeled safety height
Sorry it has taken this long to reply, been quite busy.
I am a journeyman CNC machinist, I am now retired but that changes nothing.
All CNC mills in the real world always move the X and Y axes before dropping the Z for obvious reasons.
There are exceptions but then that is coded into the GCode.
A min safe hight is ok as far as it goes, which isn’t very far, because once the X and Y is reached it slowly feeds down to start position and for every X/Y move it slowly feeds up to what the safe hight was set to be it 1 inch or 3 inches and then back down thus increasing run time dramatically.
The safe hight is to clear where Z zero is so tool does not drag.
From a G28 position the Z should move last once X/Y are reached and then rapid to the minimum safe hight.
It is one step short of what it should be.
This is standard all across the industry, CNC machines are expensive to buy more so to repair.
Thus all projects I create with Easel, which has great creativity abilities, I then export and edit in GCode editor.
Thereby fixing the bad programing, such as approach and extra moves.
This has saved me many times.
That is what I am saying.
I agree with this. The z should only move to the safe height after the x and y are already moved into place. I have ruined just 2 projects but both were because of this. Ive learned now to keep clamps out of the toolpath for the initial move but I wouldnt have to if the Z only moved once it had moved to its first X Y position.
I agree with this 100%. This was actually my very first thought after my first carve. I’ve since changed the safety height but it really does add some time to the carve.
If I may ask, how to you resolve this within your code? I would like for the machine to just home Z after the carve and leave the X and Y where they are so I don’t have to worry about hitting any clamps.
With any editor such as GCode editor or UGS platform sender.
The lines that have to be edited are Z (to the programed safe height), delete that.
Then below the X,Y move insert a new line to rapid the Z to start height.
Same at the end of the program. delete the programed Z move and rapid up to +2 inches and put that before the X and Y move.
That is how simple it is.
I ‘fat fingered’ so many Gcode programs on CNC mills and lathes and was really surprised when these people tried to tell me that what they were doing was industry standard.
I called a BS flag on that but they remain adamant.
Sample is:
From this:
G20
G90
G1 Z0.15000 F9.0
G0 X2.44937 Y5.58365
G1 Z-0.01500 F12.0
To this:
G20
G90
G0 X2.44937 Y5.58365
Z .05
G1 Z-0.01500 F12.0
See the difference? Now it moves X and Y and then drops the Z.