Good day.
I have something that has me puzzled.
Attached is a pic of a hole that needs to be cut…
the red dot is the zero of the workpiece.
Let say I have to cut the hole to 1/4" deep. Material is 1".
Then for some reason I need to cut again that same hole with 1/4" again…
I can go to the dro Z that is at 0.8 change it to 1.050 the machine will lower 1/4" for the new zero and the dro will mark again at 0.8.
the go to cut it…but since the x,y and z are moving simultaneously if I continue to go deeper the z will eventually crash into the workpiece…unless x and y moves first and then z the no crash should happen.
If I change the drawing in vcarve to a new depth it will cut air for the first part
Is there a way to accomplish this? while I am in Mach4.
I think you are talking about Rest Machining? Like if I have two operations in the same hole, so like a stepped hole. The first operation is 16mm diameter and 5mm deep. The next hole is in the middle of the first but 8mm diameter and 10mm deep?
So effectively the operation as you have it set up now, the program is written where it starts cutting from where the surface that has already been removed for the first operation (16mm dia x 5mm deep)? Thus its doing the spiral ramp down but there is nothing to cut?
If that is what you are talking about I googled “Rest Machining in vcare thingy” and got this;
Wow, that is a word salad I just wrote
Simple concept, hard to describe. It’s a checkbox in Fusion 360. Its a 24 minute video in vcarve thingy
I think it is in that direction but not it…
let see if I can explain it better.
I got a new alum bit that cuts great…I need to do a profile cut lets say 10mm deep. Since I am trying to test things out I want to cut 2 mm deep and the machine goes back zero of the work so I can inspect and the cut 2mm deep again from the last cut height and so on until I finish. that would be one of the situations…sometimes I need to cut a shape into alum and after the cut I need to go lets say 1 mm more I can change the z height in Mach4 but until an certain point.
As you have found, the first and last moves that it creates for the toolpath will travel in a straight line from the current position of the cutter to the hole, moving in all three dimensions (X, Y and Z) at once.
When you change the DRO you are effectively “lifting” the material of the table without changing the route that the cutter will take from the home position to your hole. So it eventually crashes into the side / top.
I can think of three options (I recommend the first one):
Do not change the DRO. Build a new tool path each time and use the StartDepth option in VCarve to avoid cutting air:
Set a pessimistically-large Safe Z to make the initial and final moves of the tool path go high enough to allow for changing the DRO. Ensure that this:
is something bigger than 2" by clicking this:
and changing this:
However, this option is risky if you later try the same tool path on something that is more than 2" high. Hopefully, you can see why.
Or, the riskiest option is to edit the tool path file and split the move commands in the GCODE so that it moves X&Y separately from Z. It’s risky because there will be at least two places you will need to do this and you might break something else.
Nope, Mach4 is only a runner. There is a MDI but no editor built in. Just load it into your favorite editor and refresh it. Some editors even have previews and the like.
There is an online editor that does a fair amount of simulation;
Not at all. I’m saying that it is not something that I would recommend you try when you are new to this stuff. By the wording of the OP’s question, I thought that he was unsure why the cutter was crashing and also that he didn’t know how to fix the “cutting air” thing in VCarve.
For myself, I might well edit the GCODE directly when experimenting like this, but I am comfortable with the effect of doing that and how to split the Z moves from the X & Y moves to avoid the crash.
There’s a lot of knowledge to pack into your head when you first build an AVID and start playing with it. I’ve only had mine running seriously for about a year now and I still remember how much I didn’t understand at the start.
Mach4 does have an Edit G Code button. If activated it takes you directly to a gcEdit app window where you can make Gcode changes. When you save and close it automatically updates the code in Mach4.
