Cannot move component designator

Hi everybody,

I already read this from a previous post:

I see the reported problem and there is some
unexpected interaction among the “Canvas”, “Mode footprint” and
“Highlight Net” states.

Additional information:
With Canvas “Default” and “Mode footprint”
active, “Highlight Net” must also be active to move reference
designators (hover over text, hit ‘M’ and drag text).

With Canvas “Default” and “Mode footprint” inactive, it works as
expected (hover over reference designator text and hit ‘M’ to move).
“Highlight Net” mode is irrelevant.

With either Canvas “OpenGL” or “Cairo”, “Mode footprint” state does
not matter and “Highlight Net” must be inactive to move reference
designators (left-click on text to select it and move it). Hitting ‘M’
to move will deactivate “Highlight Net” automatically.

but no matter what I do, I cannot move those designators.

In default canvas they do not pop out when i select the component. In Open GL / Cairo the designators pop out but they cannot be selected. Even if i push “M” over the designator text the mouse pointer automatically move to the center of the component and I can only move the whole component (no way to select just the designator).

I noticed on some youtube video than when this “moving designators” works, those designators appears in the “clarify selection” pop-up but in my case only track, pads, components appears there.

Using last version of Kicad 4.0.2, and I have the same problem on windows as on linux.

What I’m doing wrong?

I will appreciate a lot if anybody can help me with this stupid thing I cannot do this time.



I do not see this, at all, using a June 19 build.
In legacy mode, right mouse does not show move, but in all view modes, ‘M’ is simply always live.
Mouse Cursor anywhere inside the text bounding box, ‘M’ -> picks, snaps to centre, and moves.

Hmm, nothing I do can disable move, ie M simply always works ?
Can you post the design, maybe they are not Ref/value fields, but something else ?
If you edit in the kicad_pcb, do they change Text/location as expected ?

  (module 0805 (layer B.Cu) (tedit 577F17A5) (tstamp 0)
    (at  61.595 -22.225 -90)
    (attr smd)
    (fp_text reference R16 (at -1.143 -0.635  90) (layer B.SilkS)
      (effects (font (size 1.1557 0.96012) ( thickness 0.09525)) (justify mirror))
    (fp_text value 470R (at 1.778 -2.286 -90) (layer B.SilkS) hide
      (effects (font (size 1.1557 0.96012) ( thickness 0.09525)) (justify mirror))
    (pad 1 smd rect (at  1.143  0 -90) (size  1.524  1.27) (layers  B.Cu B.Paste B.Mask ))
    (pad 2 smd rect (at -1.143  0 -90) (size  1.524  1.27) (layers  B.Cu B.Paste B.Mask ))

BZR6971 (nightly from 7/7/2016) on Win7 64bit
…my REF/VAL fields are on F.Fab and set visible in the render tab for this.

Canvas Default Legacy :relaxed:

Mode Footprint ON
No Tool selected
REF/VAL NOT selectable and movable

Mode Footprint ON
Highlight Net ACTIVE
REF/VAL are selectable and movable

Mode Footprint OFF
No Tool selected
REF/VAL are selectable and movable

Mode Footprint OFF
Highlight Net ACTIVE
REF/VAL are selectable and movable

Canvas OpenGL

Highlight Net tool is deactivated automatically when I do anything else than selecting nets (tracks, pads).
Mode Footprint doesn’t have an influence on selectability/movability of REF/VAL fields here.

If you mean Canvas Legacy, then yes, I agree with this test. I missed the Footprint On.Legacy test.

I also find the active layer affects immediate M action, in Legacy - if the footprint is on the 'other’s side from active layer, then M is immediate, if it is on the same side, you get the pick-choice.

1 Like

I opened an old project I was working few months ago and I found that on this project the designators can be moved. During my investigation I noticed also that they are visible without clicking on the component.

Knowing this I decided to open the kicad_pcb file and compare the two project files.

I found option visible_elements was different and so I changed it from
(visible_elements 7FFCEF7F)
to the value set on the old project:
(visible_elements 7FFEEFFF)

After this just reloaded the kicad_pcb file and now designators are visible and can be moved like the old project.

I download this kicad_pcb file from some reference design and used it as base for my project, so I don’t know how this option got changed. I played a lot with visibility options, but cannot figure out where I can turn on or off this designators.

It is my understanding that if designators are not visible they cannot be moved … don’t know if this is a bug. Let me know if I need to open some bug, it may help someone else to have it fixed.

Under Render.Values & Render.References, I can change
a (visible_elements 7FFFFFDF)
b (visible_elements 7FFCFFFF)
c (visible_elements 7FFFFFFF)
b is Ref,Value OFF.
c is all Render options ticked.

Found it … and yes if I disable “References” I cannot move those anymore.