Problem with engraving cutter

[racerbear]

Good afternoon all

I have a problem with a 45 deg engraving cutter which is quite bizarre, at least to me.

I used the tool base in aspire to set up an engraving cutter as shown in the screen grab

Tool setup in tool database

which information I then used for a v-carve cut as shown on second screen grab.

Tool set up in Vcarve

When the cut was completed, the finished depth of cut was 2.34 mm.

I ran it again to ensure I had not done anything daft, but achieved the same result. Just to check, I ran the same v-carve profile but changed the cutter to a ball nose 2mm and the depth of cut was 1mm.

Does anyone have any bright ideas here, as far as I can tell the cutter is correctly set up in aspire, I used feeds and speeds from Gwizard, have I missed something obvious in the tool set up?

As usual all answers gratefully received.

[Alan Male]

Might have nothing to do with it, but you have 'Project Toolpath on to 3D Model' selected?
Is it necessary for this job?
Cheers....
Alan

[TReischl]

What depth does your CNC code show? You know, the Z value.

If your Z depth is -1.00 then the program is operating correctly.

There are some people who firmly believe they should not have to be able to read CNC code, like it is somehow beneath their dignity or "the software takes care of that why should I worry?"

But, something like this is EXACTLY why it pays to be able to read a bit of CNC code. Within a few minutes you would be able to tell if the software was performing correctly or if there was a different problem.

[TReischl]

Might have nothing to do with it, but you have 'Project Toolpath on to 3D Model' selected?
Is it necessary for this job?
Cheers....
Alan

Ran a quick test and the "Project. . ." does not seem to have any effect on depth of cut.

[scottp55]

I noticed you were projecting on to a 3D.
Depending on the shape of the 3D, when you hover over the toolpath it will show depth from top of material...not actual depth cut into the 3D.
It's still a VCarve so depth will be changed by the shape of the bit if it can't get all the way to your flat depth.
Just to double check myself, I did this quickie with both a 30 engraving and a 1/16" TBN.
For the 30, I got a max depth of .5354"
And the Tapered Ball Nose was .4818"
Even though flat depth was .1" for both.
Without seeing the 3D, I was wondering if that might be the problem?
IF it was an actual measurement from a finished cut...Then I'm stumped why the engraving bit carved to deep into your material.
I see other people have mentioned it also while I was drawing, but posting anyways.
scott

[racerbear]

G code shows -1 in all cases which is why I think the problem lies within the tool database setup somehow........

The dimensions I gave are finished cut depths after a completed cut.

I thought the project on to 3d was only for visualising the design?

[Adrian]

If you're not cutting onto a 3D model then turn off the Project onto 3D. It can cause all sorts of problems with 2D toolpaths so it's best to make sure it's off unless you're really using it.

If your gcode is showing a maximum cut depth of 1mm but the actual project is cutting to more than that on your machine then it's not the tool database or Aspire that is wrong it's something with your machine or controller software.

[racerbear]

I measured the z axis travel against a known size block of steel, and it was within 0.02mm

The exact same path cut with a 2mm dia ball nose tool cut to 1mm depth, again within a small margin, it is only the engraving tool that seems to be causing problems, which is why I thought it was a problem with the translation through the tool database.

If you set up a Vee bit, you set the included angle for the tool point, but with an engraving tool, you set half of it according to the illustrations on the set up, could this possibly be a bug? I forgot to say this is Aspire 4.5, sorry.

I will try turning off the 3d and processing it again, and then compare the code, if it looks different, I will run it and see what it produces, but like I say, with both tools, the Gcode shows a cut depth of 1mm

[racerbear]

I just compared the 2 sets of code with and without the 3d

With 3d it produce 17461 lines of code

Without 3d it was 14961 lines of code

I will run it tomorrow and see what happens but I did not se anywhere on the 3d code that showed a cut below 1mm

[racerbear]

OK, I ran the modified, i.e. without 3d selected, file and it was still cutting too deep, it was however a slightly shallower cut than with the 3d selected.

I checked the calibration of mach3 using their suggested method and it was virtually spot on, as near as I could measure, for travel in the z axis actual against the commanded movement.

I also tried changing the tool angle to 45 degrees on the engraving tool just in case it was some error in that respect, and ran that, same result.

I am now very confused, not difficult I know. any further bright ideas please ??

[TReischl]

G code shows -1 in all cases which is why I think the problem lies within the tool database setup somehow........

The dimensions I gave are finished cut depths after a completed cut.

I thought the project on to 3d was only for visualising the design?

If the g code is showing the max of -1 then there is something going on with your machine or the way you are setting it up. The g code runs the machine, not the tool database setup. When you are only commanding a max depth of -1 in the g code and you think the database is causing a problem is beyond me. The machine controls knows nothing about your tool database.

Think about it, -1 is -1 is -1. There is no secret command in that G code telling your machine to go deeper.

How do you set your Z zero? The tip of the tool should just barely touch the surface of the workpiece when the Z axis reads 0.

Attach as much of the g code as you can and we can all take a look to make sure you are not missing something. If we see a Z depth greater than 1, then it is a software issue, either a bug or operator error. Big hint here: Bugs are extremely rare in this software. Also, you are doing a very common operation that is done countless times everyday by other users. Sooooo, the odds of it being the machine or what you are telling it causing the problem are very good.

BTW, quite a few folks set Z zero by using a .5 block of brass/alum, then key in .500 to the Z value. How are you doing it?

[racerbear]

OK, that is why I am asking the question here because I am at a total loss.

I am new to this world but have followed the setup instructions and as far as I can tell the axis travel is correct, I followed the instructions for checking, and the travel actual was, within my abilities to measure, the same as the travel on the code when I ran the setup instructions.

If the g code is showing the max of -1 then there is something going on with your machine or the way you are setting it up. The g code runs the machine, not the tool database setup. When you are only commanding a max depth of -1 in the g code and you think the database is causing a problem is beyond me. The machine controls knows nothing about your tool database.

I know that, which is why I am confused, when I run a pocket or profile with another tool, 1mm cut on the code is 1mm cut actual.

How do you set your Z zero? The tip of the tool should just barely touch the surface of the workpiece when the Z axis reads 0.

I use the zero setting tool which came with the machine, however I have checked it manually, and it is correct, the tool just touches the work at 0 on z axis.

File added as requested

moto_ducati_45deg_1mmcut_carve.txt

(222.01 KiB) Downloaded 225 times

I know it is what is done 1000's of times a day, which is why I need help to get it right


Thanks again in advance,

[TReischl]

Read through the G code, nothing wrong with it that I could see, no Z moves that would produce the overcut.

In the beginning of the program there is a line with an H1 in it. H is a tool length offset.

Here is the thing, if all your programs have that H1 in them then they should all work identically in terms of depth of cut. But, if you have input a value for H for only this program it would cause you trouble. It should be set to 0.

Frankly, I do not think that is your problem but it is something to check to eliminate one more possible cause.

If you run the program with a different cutter, like a small end mill you should get the same depth of cut. The machine actually has no idea what cutter is in the collet.

If something is loose in your Z axis, it will not always show up with all cutters. Different cutters put different forces on the axis.

A good question is "If you manually position the Z axis to zero after running the program, is it actually at 0 or has it changed?"

After looking at your code I am confident you are not having a software problem.

Curious, what machine are you running?

[Mobius]

The problem is evident in your Gcode file. Line N14 contains a G43 tool offset command of 20mm. This is linked to the specific tool number you used for this tool. If you delete this line in the Gcode file your bit should cut normally.

I recommend removing the G43 line from your post processor to avoid further issues. The only time you would need a G43 command is if you are using a auto tool changer where the bits have a consistent preset length. If you use a touch off method, G43 is not necessary.

[TReischl]

Mobius: I missed that one!

But, that is 20mm which is a whole lot more than the error he is encountering, but maybe coupled with H1 who knows?

I agree with you about removing the line entirely. I went through my post and got rid of all sorts of startup code that was not necessary for the way I run my machine.