Paint issue

[Tung Bui]

When creating custom polygon and choose paint, it doest allow to choose cut-z, i think it’s better when there is a checkbox “auto” to let user switch between automation and manual mode, as picture, when my dia param is 0.5, it doest allow to change z-cut, also, the gcode generated is empty too. (as my machine, the smallest diameter after milling is 0.4-0.5 what ever the tooldia is 0.1mm). and there is one thing i can’t understand is the depth milling of the small diameter will deeper than the big V knife, as the result calculated in the image 2, i guess the tip 0.1mm will be broken when milling at 0.35mm depth ( i have not try it yet ), on some board with the thickness 0.5mm, perhap it is a nightmare

‌

The second:

when change tool to 'C' tool, it is work, but there is a small problem as picture bellow, the green is the area will be paint, but it overlap the boundary of the geometry

‌

‌

[Marius Stanciu]

Hello,

The idea is that when using a V-shape tool the program always assume that you are going to do engraving. The reason for having the Cut Z parameter grayed out is that for a V-shape tool the depth of cut (Cut Z parameter) depends on the: cut width (the tool Diameter in the Tool Table), the V-tool tip diameter and the V-tool tip angle. Since the V-tool tip diameter and the V-tool tip angle are fixed (for the chosen tool) the user can either change the cut width (Tool diameter in the Tool Table) or the cut depth (Cut Z parameter).
So you might wonder why we don’t change the Cut Z parameter for a V-shape tool and we don’t have the Tool diameter (in Tool Table) grayed out (and automatically changed) once the Cut Z is modified.
That is because the distance between tool paths, the cut with (tool diameter in Tool Table), is not something you can change when doing milling. Your Geometry object, the one you are milling, was created in Isolation Tool (plugin) (or Paint Tool, NCC Tool) using a certain tool diameter.
If you use a different tool diameter when milling then the end result will break the isolation assumption: that the features that were isolated are protected by isolating at a certain distance.

In short this is the reason why you can’t change the Cut Z parameter when using a V-shape tool. That is because you made the decision in a previous step on how much should be this tool diameter.

But if you want to overcome this limitation, and if you assume the fact that there will be excessive cuts, then you can change the Tool Type from V to any other (like C…). You can still edit the tool diameter in the Tool Table (double click the diameter value) and that will adjust the cut width.

For your second issue: the red lines are tool paths. The endmill center will follow those lines and you will have half of the cut to left of the tool path and half of the cut to the right side of the tool path.
If all the paths in your picture are one Geometry object then when the milling is done the above will happen. If the outline is a different Geometry object, you are milling the painted object there is nothing to make the milling aware of the initial outline. It is your responsibility to make sure you use an appropriate Offsetparameter and Overlap parameter in the Paint Tool (plugin) when you are doing the painting.

Best regards,
Marius

[Tung Bui]

I think automation calculate Z depth is something wrong, that isn’t what user want to do. there are several thing as bellow:

1/ user cannot change V-shape diameter, if i buy a v-bit 3.175”, 0.1 diameter 60 deg, then i cannot change it

2/ the depth milling is what user will input and your tool calcule effectly diameter instead block user input the Z value as image bellow

‌

now, the problem is: if i want to milling down 0.1mm depth, i must calculate effectly diameter, in this case is 0.2155mm and input it to flatcam while isolation route as bellow

‌

and at second screen i should input as bellow

‌

so i think the right way is:

1/ user input tool flute diameter (eg: 3.175”)

2/ user input v-tip diameter (0.1mm)

3/ user input v-tip angle

4/ user input z-cut as he want (0.1mm)

and your application will calculate effectly diameter (0.2155mm - if i want to milling down 0.1mm) (user can choose to input this value manual too because the cheap cnc and cheap vbit cannot milling exactly at 0.2155mm) and generate the isolation geometry for the cutting. It is rarely to milling down more than 1.6mm so input tool flute diameter (3.175”) isn’t neccesary but if you want your software support to milling anything right way, then implement it :D

‌

bts: instead input something complex like that, i think create tool table for the popular tool is better, it will have all that properties flute 3.175inch,10 or 20 or 30 or 60 or 90 deg, and tip diameter is 0.1 or 0.2 or 0.3. Or at least user can create his own tool and save for later using without re-input what ever he open flatcam application

[Marius Stanciu]

Hi,

Ok, I will try to make it simple:
1. You use the Paint Plugin (Isolation Plugin, NCC Plugin), to create the isolation paths. At this point in time you decide what tool you are going to use, the physical dimensions of the milling bit. If you use a V-shape tool you have to decide now what is the isolation distance and what is the depth of cut into the PCB material. Due of the tip diameter, tip angle and isolation distance you will get a real tool diameter. The end result will be a set of isolation paths found into a Geometry object.
2. Milling step. In the current version it is done in the Geometry object tab. In the next version it will be done in the Milling Plugin. Even at this stage you can still edit the tool diameter. Why? Because it is possible and someone might want it. Otherwise you have no reason to change the tool diameter in this step (by changing the tool type from say C1 to V) because the decision on what will be the depth of cut (Cut Z parameter) and what will be the tool diameter (calculated for a V-shape tool) was done in the previous step. The reason why you can still make changes to the tool diameter is that there may be other applications for the Milling Plugin since FlatCAM beta is no longer a PCB milling software as it used to be.

This is how the flow of the software is and it will be, because it makes the most sense and it offer the maximum of flexibility. Anything else will mean a radical change in the software and weeks of programming.

[Tung Bui]

ok, i understand it, from here “you have to decide now what is the isolation distance and what is the depth of cut into the PCB material”, i think you could automation calculate “isolation distance” when user input Z value, it will be simple simple as “C” tool, except the “isolation distance” will be changed when the Z depth changed.

[Tung Bui]

too complex

[Tung Bui]

done