Bulk modify for parallel lines (or similar parameters)

[cgherghe-2]

Is there a way to bulk modify certain parameters when sketching?
For example, I have four parallel lines, and I want all of them to be 20 mm apart (equidistant).

I was hoping to be able to select/highlight all four lines (or the dimensions), then click on the NORMAL button and change all four dimensions in one stroke (please see picture attached)... 
Unfortunatelly, it does not work like that -- for four lines it is not a big deal, but if you have hundreds of these lines to align like this, such a shortcut would be a tremendous productivity trick!

P.S. I chose the label forced by the system, could not find a SKETCHING label so I took the one that sounded close...

[tbraxton]

I don't think the solution you are wanting exists within sketcher as you would like to have it implemented. You can select many dimensions at one time using box select method and then select the modify dimension function to modify multiple dimensions at the same time but you must enter a value for each unique dimension.

To Modify a Group of Dimensions

1. Click and drag a box to select one or more dimensions to modify.

2. Right-click and choose Modify from the shortcut menu or click Sketch >Modify.

The Modify Dimensions dialog box opens. Each of the entities and the dimension values you selected appear in the list.

3. Set any of the following options:

◦ Regenerate—Click the check box to regenerate the section every time a dimension is changed. Clear the check box to regenerate the section only when you have finished modifying dimensions.

◦ Lock Scale—Click the check box to lock the section scale. Clear the check box to allow scale changes.

◦ Sensitivity—Drag the slider to change the sensitivity for a selected dimension.

4. Type new values for the dimensions.

5. Click OK. The section is regenerated.

You can also constrain the dimensions to be equal but I do not think that box select works with that function so you will have to select each dim with the mouse.

You can copy and paste sketch entities where move/scale/rotate functions are available.

You could also use the pattern feature to space lines at regular intervals but not within sketcher.

Look through this thread and particularly the video posted for an example of how to deal with equidistant spacing of lines used to create a scale hash pattern.

https://community.ptc.com/t5/3D-Part-Assembly-Design/text-repetition/m-p/697334/highlight/true#M74160 

[cgherghe-2]

I will look at the thread and watch the video, thank you!

[pausob · Accepted solution]

There are things in Creo sketcher that can be done in bulk, but I haven't seen dimension being auto-applied in the manner you described.  What about using construction lines to space things apart evenly?  Those can be made "the same" by bulk-selecting and applying the 'equal', parallel, horizontal, vertical and converting to construction, etc:

(the left-mouse-button popup menu does record properly on my system, so I'm using the right-mouse-button menus when recording the above clip)

[cgherghe-2]

I will try it out, thank you!

[KenFarley]

When I have several lines I want to be parallel and equally spaced, this is my trick for doing it so I only have to change one dimension to change the spacing:

(1) Draw all the lines, making sure they're parallel. Don't care about the spacing at this point, don't put any "real" dimensions on any of them.

(2) Place a convenient construction line that is perpendicular to this array of lines. Might be from an endpoint, might be the midpoint of one of the outermost lines.

(3) Define construction circles that have their center on that construction line, one between each set of the parallel lines. Make them all equal size - Creo makes this pretty easy.

(4) Dimension one of the construction circles.

(5) Make each of the parallel lines tangent to its adjacent circle(s).

Now all the lines are parallel and equally spaced. to change the spacing you only need to edit the dimension for the one dimensioned construction circle.

I use this technique a lot for defining "offset" geometry that isn't amenable to the normal offset functionality of the sketcher. It's somewhat tedious to implement, but has worked dandy for me.

[cgherghe-2]

Now this is a nifty trick, pure geometry at work! Nice one, I will try it out, thank you!

[Pettersson]

You can also set an equal constraint on the dimensions. click the equal constraint, then click the dimensions one at a time. they will all be constrained to being equal, and you can then edit only the first dimension and have them all follow.

Of course, if you have hundreds such lines, generally it's advised to not do them in the same sketch, but rather see if you can't do what you're trying to do with a pattern instead.

[cgherghe-2]

I did try the equal constraint on the dimensions before posting here, but obviously I did something horribly wrong because it did not work at all for me... I will try it again following your instructions, thank you!