LinuxCNC Features - a kind of NGCGUI

hi guys,

I've been using features almost a year now, and i love it. Great work you have done here! It is developing really well.
I just wanna inform you about a few bugs i found in latest version:
- Spindle is always set to 1000 rpm, no matter what i type in tool change - altought the final spindle velo is ok, it changes speed when cutting last cut.
- feature "slot" doesnt work ok - the dimensions of the cut are not the same as dimensions entered for height and width - I suppose there is something wrong with tool radius compensation calculation
- cutting from positive Z to Z>=0.000 doesnt work - it says invalid cutt depth.For example if you set your Z zero on the bottom of workpiece and you dont want to cut trough it.

And leave spindle as it is, turn on with the first move approaching start point, turn off at rapid Z at the end of program. On a big machine like mine it takes several seconds to get the spindle to speed, so constant turning on and off is not OK.

Hi,

Thank you very much for your very important comments, this is really needed for improving. I would really like more.

fixer wrote: hi guys,

I've been using features almost a year now, and i love it. Great work you have done here! It is developing really well.
I just wanna inform you about a few bugs i found in latest version:
- Spindle is always set to 1000 rpm, no matter what i type in tool change - altought the final spindle velo is ok, it changes speed when cutting last cut.

It's an unfortunate oversight.
In fv_tool-change.ini add this new line after "F#param_feed"
#<_spindle_rpm> = #param_speed

fixer wrote: - feature "slot" doesnt work ok - the dimensions of the cut are not the same as dimensions entered for height and width - I suppose there is something wrong with tool radius compensation calculation

Tool radius compensation is calculated by LinuxCNC, so I guess this is OK.
The width is the diameter of the arc and the length is the distance between center of arcs.
As for now I can not use my milling to test. I will follow up when I can.
By the way, is the diameter in your tool table for the mill you use the right one ?

fixer wrote: - cutting from positive Z to Z>=0.000 doesnt work - it says invalid cutt depth.For example if you set your Z zero on the bottom of workpiece and you dont want to cut trough it.

I changed it for the new release to come but if you need it NOW here is what to do.

The files that need to be edited are in lib directory : fv_circle.ngc, fv_ellipse.ngc, fv_polygon.ngc, fv_rectangle.ngc, fv_slot-arc.ngc, fv_slot.ngc
Find the block that says : if [#<cut_depth> EQ 0.0]
Replace it with : if [#<cut_depth> GE #<cut_start>]
Delete the else condition and the following line keeping the the last line of the block, the one that says "endif"

You will then be able to use any number as long as "cut depth" is lower than "cut start"

fixer wrote: And leave spindle as it is, turn on with the first move approaching start point, turn off at rapid Z at the end of program. On a big machine like mine it takes several seconds to get the spindle to speed, so constant turning on and off is not OK.

I agree

I will have a new release in a few weeks with many improvements to make it much easier to use.
There are changes in the subroutines and a few new one to come.
If there is something specific you would like to see added, tell me about it

A few screen shot of things to come. Please comment





Menu is reorganized and include many accelerators/shortcuts


Better grouping makes it easier to use. Single view is default now

Best regards
Fern

ok, thanks for the updates,
regarding slots, i am not sure but i belive that the problem was that, as you say, the length is between centers, and i was wrongly expecting value between arcs...

I am working on a subrutine for features for cutting out shapes for common d-sub connectors in enclosures. Not what every machinist would need, but there are quite a lot of electro guys with CNCs, I am sure someone will find it useful. I will post it here tomorow, if everything goes OK.

I would also like to propose a small change in GUI: Can you make the Add feature window to not be additional window, but would show the menu in the "value" part of the main window? After you would choose feature to add it would disapear and normaly show values as before. I am using touchscreen and it is not convenient to have additional windows on top of main.

And with touchscreen, taping on a feature or folder doesnt open it, it only selects and i have to press enter to open/add it. Can you do an option for adding a feature with single/double click? User with mouse will propably want double click.
A small popup numerical keyboard wich would show when selecting a value is propably too much to ask, a?
I am learning python, but curently i am not good enought to make that kind of changes in your program...

and you can hide the shortcuts for features, as i personaly never use them, and make upper icons bigger, again because of touchscreen being inacurrate...

As promised, subroutines for D-SUB cutouts. Dimensions for connectors are hardcoded in metric, use tool no larger than 3mm. For imperial units, just recalculate hardcoded dimensions in lines after 17 in ngc, or change into metric before subroutine call with custom G-code.

You can include them in final, but i see no point in this because very few people will find it useful. We could make repository or a new topic for collecting diferent subroutines, what do other users think?

Finally started to use the Features for conversational programming.

Using FernV-linuxcnc-features-388af08.tar

Just to let you guys know, I, too, have the spindle set to 1,000 rpm, even if I ask for 2,000 rpm in the ToolChange window.

Using mill-mm, at about line 23 in the ngc file I have:

#<_spindle_rpm> = 1000
#<_final_spindle_rpm> = 1000

Then, later I have:

...
o<toolchng-001-ena> endif

S2000
F100.000

#<_final_feed> = 75.000
#<_final_spindle_rpm> = 2000
#<_ffeed> = 100.000
#<_vertical_feed> = 25.000
#<_plunge_down> = 0
#<_depth_step> = -0.500
#<_plunge_ratio> = 0.07
#<_pocket_ratio> = 0.80
(End tool change)

I wonder if the #<_spindle_rpm> should be set to 2000, and <#_ffeed> should also be set?

I'm ONLY boring circles out; the final cut does indeed go to 2,000 but all cuts to then are at 1,000 rpm.

Thank you!

Hi Johns,

The solution is in the post #62149

Here is the easiest way until I post an update

1. Right-click on Tool Change in the top treeview and select 'Edit Current Feature'. It should open fv_tool-change.ini in gedit
2. Go at the end of the file and add this new line after "F#param_feed" : #<_spindle_rpm> = #param_speed
3. Save the file
4. Right-click again on Tool Change in the top treeview and select 'Reload Current Feature'. It will load the updated version.
5. Edit the values with the ones you entered before
6. Delete the old one

The change is permanent

Regards
Fern