8.994 creates zero depth cuts in CNC job.

Issue #531 new
Terry Jones created an issue

I was getting strange results using 8.994 and went back to 8.993 and things started working.

Using the isolation tool in 8.994 and examining the GCode shows Z is always 0.00 instead of the Cut Z depth of -.08 as specified in my preferences.

I made sure my Cut Z was -.08 in prefs in Geometry Create CNCJob and in Tools Isolation Tool.

None of my Cut Z values are zero. But for some reason when I look at Tool Data Cut Z is 0 in CNC Job Object Properties (see attached pic)

Comments (6)

  1. Marius Stanciu

    Hi Terry,

    Thanks for the donation! 🙂

    Regarding your problem, it is possible that when you were in the Isolation Plugin (Tool) that you have selected a V-shape tool and:
    - the Tool diameter in the Tool table was say 0.1mm
    - the V-tip diameter (which is the tip diameter of the v-shape tool) was the same as the tool diameter (in our case, 0.1mm)

    In this situation the application will calculate automatically the cut depth (Cut Z) and adjust it regardless of the settings you made in the associated field. And with both those parameters the same value (0.1mm) the calculated Cut Z value is 0.0 due of the shape of the tool.

    The fix: There is a Calculators Plugin (Tool) in the Tools menu where you can make the V-shape calculations yourself and then in the Isolation Plugin (Tool) you no longer select a V-shape tool but a “Cx” (circular cu x teeth's) and then write down the Cut Z and edit the Tool diameter in the Tool table to the calculated value in the Calculators Plugin (Tool).

    Best regards,

    Marius

  2. Terry Jones reporter

    Received email and tried to reply… bounced

    ----- The following addresses had permanent fatal errors -----

    issues-reply@bitbucket.org

    ‌ (reason: 550-5.1.1 The email account that you tried to reach does not exist. Please try)

    Here was my reply

    I am struggling with this tool stuff...

    I get that a V tool that has a .1 tip width and 30 degree shape will be wider as it goes deeper.

    I guess I figure if I tell the program its .1 tip diameter and 30 degrees it should figure the rest out based on Cut Z value. The deeper the cut the wider the tool at the top... so not sure why there is a new diameter field that has to be filled in manually...

    Also just checked my prefs and I appear to be set to Tool Type Circular not V.

    Not really sure what circular means either... is that ball shaped or flat endmill shaped? A V tool is v shaped looking from the side so circular implies circular from the side thus ball shaped tool.

    But there is still something buggy in there aside from my total lack of understanding,...

    I do what looks like the same thing two different ways and get two results... Here is how I am reproducing both repeatedly in 8.994

    Method one that generates bad code

    Open gerber

    Double click on gerber in project which brings up properties.

    In properties I click on Isolation Routing button which brings up the Isolation Tool with V tool selected .1 dia

    I click Generate geometry and get the Geometry Object showing Cut Z as 0.0 and greyed out (as per tool tip)

    I change tool type to C1 which changes Cut Z to -.08

    I click Generate CNC job and then view the Gcode and I see zero depth

    Method two which LOOKS the same but generates different (correct) gcode

    Open gerber

    Double click on gerber in project which brings up properties.

    In properties I click on Isolation Routing button which brings up the Isolation Tool with V tool selected .1 dia but this time I change to C1 here and click Generate Geometry and the Geometry object here looks identical to the one from method one (Cut Z -.08) so I click generate CNCJob Object

    Examine the code and Z is -.08

    So given that the two Geometry Object panels look identical to me I would expect the CNC code to generate the same.

    May be unrelated but I do not understand the Cut Z value in the Geometry Options in Preferences. Why is there a Cut Z value in the geometry?

    TJ

  3. Marius Stanciu

    Hi Terry,

    Received email and tried to reply… bounced

    The email you received is sent automatically by Bitbucket whenever somebody is writing in a Bitbucket section where you are set as “watching”. Since you created this issue you are also automatically added as a watcher of this issue and receive emails when someone post in here. Those emails cannot be answered to, you need to come back here and post a reply.

    Since the release of v 8.994 I worked a lot on the app and what is now almost v 8.995 is a very different thing. Even the UI is changed. What I want to say is that many issues that were present in v 8.994 are now solved for the next version.

    Also the idea is that starting with v 8.992 I began to make structural changes in the app which in turn created a lot of bugs. That is the reason for what you see in the 8.994 and the reason also for the delay for 8.995 (soon will be a year since the last release).

    Now, we need to clarify a few things.
    1. The Isolation plugin allows you to add more tools in the tool table. E.g writing 1.429 in the Tool Dia field does nothing until you hit the Search & Add (or Pick from DB) button. At that moment in time you will have 2 or more tools in the Tool Table and therefore will create two sets of isolations in the same GCode file (at a different distance from the trace depending of the actual diameter of the tools).
    [Bear in mind that this is not rest machining, they are done without awareness of one to the other. When you activate FlatCAM Advanced mode (in Preferences) then you will be able to use Rest machining which means that using multi tools, the bigger tools take its shot at doing the isolation and smaller tools will try to isolate where the bigger tool could not and so on until there are no more tools or the isolation is finished.]

    If what you want is to change the diameter of the tool you just use the same technique that you are using in operating system (use a delayed double click or the F2 key) over the tool diameter column in the Tools Table.

    1. In the Isolation Plugin the most important parameter is the isolation distance, the distance between the actual toolpath and the geometry that is isolated. That is the Tool Diameter from the Tool Table.

    Because of that, when you select a tool type: V-Shape, the fixed parameter is the tool diameter (from tool table) because it shows that distance that is chosen depending on the clearance you have in the Gerber object between any two geometric elements.

    So it’s fixed. But due of the shape of the tool the other tool parameters are: tip diameter, tip angle and Cut Z (depth of cut).
    You need to play with those to get the desired depth of cut (Cut Z) but most of the time the tip diameter and tip angle are also fixed (because there is a limited number of combinations and also there is also the problem that you may have available only some of those tools at hand) which leads to the fact that the Depth of Cut (Cut Z parameter) is now the only adjustable parameter so it is the end result of what you choose in the other parameters.

    Bottom line is that in Isolation Plugin, the Depth of Cut (Cut Z) for the V-shape tool is automatically calculated. I know that your intuition says that you need to adjust the Tool diameter (the distance to the traces/pads) and not the Cut Z (because going deeper will damage the tool faster) but because of the constraints: it is paramount to maintain the Gerber geometry unaffected ,that’s the way it is set to work like this.

    The reason of why there is a Cut Z parameter in the Isolation Plugin (Tool) is because for the V-shape tools it make sense to become aware at this step (by checking the Cut Z parameter) if the isolation job will be what you want or not. Those values are supposedly inherited in the next phase when you generate the CNCJob (in 8.994 and versions before that, this happen in the Geometry tab, in the next version there will be a Milling Plugin that do that).

    Not really sure what circular means either... is that ball shaped or flat endmill shaped?

    Circular tool means that the diameter is constant from top to bottom of the drilling length as opposed to the V-shape tool which has a “tool diameter” that is progressively greater as you go deeper.

    Best regards,
    Marius

  4. Log in to comment