dragging dimensions in edit mode

[EA_8293306]

Hi,

How do I drag dimensions while in edit mode like this:

https://www.youtube.com/watch?v=kRxBD-B5IrY&t=49s

I attached a gif of me trying to drag sketch dimensions.

 

it doesn't matter if dimensions are weak, strong or locked.

I'm currently using Creo 8.

thanks

[StephenW]

You can drag within the sketch or the dimensions can't be locked (i think your green dimensions are locked (rmb unlock on the dimension)

[EA_8293306]

the dimensions are not locked. 

look at the new gif i attached.

I remember being able to do it when i worked with creo back in 2019...

did they change something?

[tbraxton]

They are dragging a dim of a sketch of the feature shown being flexed viewed in 3D. You can activate the sketch (modify dims) via the model tree to access the drag handles and dimensions while in a 3D view. Activate the sketch to show the dims and you can then LMB to select the sketch elements and drag.

@StephenW has noted that if the dims are locked in the sketch, then you would not be able to drag them. It looks like he has identified the issue you are having.

See this video. 

drag sketch.mp4

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[EA_8293306]

this is exactly what i am trying to do .

but i cant grab the dimensions.

i attached another gif

[tbraxton]

This may seem obvious, but I must ask. Do you have your selection filter set to dimensions when you are trying to select a dim for dragging?

[EA_8293306]

tried this. didn't help

[tbraxton]

I have a custom mapkey that sets the selection filter to dimensions for this very reason. This is why my edit dim icon looks different than OOB. Creo does not set the selection filter to dims when using the edit dim command (I have asked them to fix this for several years).

[kdirth]

Getting the drag handle for a dimension is a bit difficult in edit mode.  You have to hover the mouse into an annoyingly small space over the arrow to get it show.  Dragging the lines, arcs, points, etc. is much easier.

dragging

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[EA_8293306]

i can only grab the dragger for the extrusion, not the drawing dimensions/line/curves

see gif 

is it something in the config file?

[tbraxton]

Try selecting the numbers in the dimensions rather than the arrows and report back if that works. I am testing this in Creo 9, not Creo 10.

[tbraxton]

I do not think this is related to a config setting but I would not bet my life on it.

I have noticed that it appears you are using sketches external to the features you are attempting to dynamically modify. This is probably the reason that the behavior you are observing is "different". Try creating a feature using an internal sketch in your test model and see if that behaves differently.

[EA_8293306]

using internal sketch didn't help

 

[tbraxton]

I am out of ideas for the root cause of the issue at this time. If you are using a commercial license, post one of you test models here. We could then have the chance to open the model and test for this behavior.

[EA_8293306]

I attached a sample file.

thanks

[StephenW]

@EA_8293306 

Don't use the dimension to drag, use the highlighted sketch edges to drag, the slightly different color orange edges.

[EA_8293306]

first of all, thank you for taking the time to try and help.

unfortunately nothing seems to work. It doesn't matter if its an extrusion, revolve or just a sketch on its own.

I can drag feature dimensions (extrusion length, shell thickness, ect.) just not sketch entities

I tried:

1. grabbing the sketched lines and not the dimension arrows.

2. using internal sketches.

3. selecting dimension before dragging.

4. having the selection filter set to "dimensions".

I made sure all dimensions are either weak or strong (not locked).

maybe its a bug with the specific version  (8.0.4.0) we use at my company because  other engineers here  (the 3 I asked) are in the same situation.

I worked with Creo up until  Jan. 2020 and I remember being able to to this. 

 

[StephenW · Accepted solution]

Maybe a bug, more likely a setting.

Try temporarily removing all config files. I typically just rename them with an X in front, but you can do it however.

Then restart Creo and retest. This will give you and "out of the box" test with no options set.

You can find all your config.pro files under file options configurations editor.

[EA_8293306]

Thank you!

the config file had "sketcher_3d_drag no"

its working now

[StephenW]

I'm on creo 6. 

I can drag the geometry if the dimension isn't locked. I am specifically selecting the geometry, not the dimension.

See video

[EA_8293306]

tried that as well. didn't work