How can I keep my selection after using offset?

ChaosCrafter

I'm trying to do a complex design that requires 4 lines to be offset from a master line.  
Because the master line crosses itself many times, I can't select the entire line and even using the make selection options isn't helpful.
Once I select the set of line segments (usually 10-12 segments including some that require zooming to even find them) I want to use next, I can offset happily, but as soon as I do the lines are unselected.
Is there any way to automagically reselect the lines I previously had selected?
Alternately, is there any way to do multiple parallel offsets (for example, putting comma separated offset values as in  offset by 7,5,-5,-5) or to select a line to the last selectable link before offset isn't viable (offset won't run through crossovers)

NeilCooke

With the sketch offset command, click&drag will select the entire chain of elements. This does sound like your sketch may be getting too complex. If you share the URL to your doc we can take a look and perhaps suggest a better way?

ChaosCrafter

Many thanks for the quick response.
I'm not sure simplification is viable.  The pattern is a celtic-knotwork rose (currently, it's not quite right and I need to be redo it as I've lost some freedoms and locked it in ways I don't want)
Here's the link.
https://cad.onshape.com/documents/0e684e8330725a73e3280e62/w/151820cd2ddbe6a83033c8c9/e/176f8bcfae4bf43bcae5ef50
Sketch 1 is the construction lines that provide all the mid-way line I'm expanding
Sketch 2 is the basic construct completed, but I've limited ability to modify it because of the work involved in setting it up
Sketch 3 is sketch 2 copied where I've started breaking line segments and pinning to complete the knot-like aspects of the final product.
The approach I'm using is to define the centre line for the paths, then extend them by #width/2 on each side to provide a channel of #width, then to add further construction lines at #width*0.75 to provide the cutting lines that make the segments go over/under each other.
Comparing Sketch2 and sketch3 will help that make more sense.
If I could, I'd have the ability to group lines into named groups, and the ability to produce offsets that crossed themselves.
Even just offsets that crossed themselves would be enough for some of it, and alternately, multiple parallel offsets would be good.
Finally, as a least good option would be a key combo that recalled either the last selected set of objects or the last saved set (with the assumption then that another combo saved them.)
BTW, is there any way to do the equivalent of trim, but to convert segments to/from construction lines?  Otherwise my changes have to be destructive (cf sketch 3 vs sketch 2) - I'd like to keep the final sketch version bound from the initial parameters so I can adjust the layout to my satisfaction.

P.S. Count me as another vote for being able to choose the colour and width of construction lines and of final lines - preferably also letting groups of construction lines be coloured differently

romeograham

Hi @ChaosCrafter

This is a situation where complex sketches can be avoided, and you can leverage the multibody capabilities of Onshape. You're right, all the self-intersecting areas are problems for sketches - but no problem for Boolean operations.

Here's my Copy: https://cad.onshape.com/documents/55b0a16cbce6cd863b66bb79/w/773f47e393e1cbb5488c13af/e/6fe7b1158e7a824400a93091

First, note the symmetry in the design, and make a sketch that only contains the elements you will pattern / mirror later:


Then, Extrude the important lines as surfaces. Because of the self-intersections, several features are needed:



Next, Thicken the surfaces to end up with intersecting bodies:



Once you have Solid bodies to work with, you can then use the Boolean - Subtract feature, with Offset to create the various "overlapping" features:



Once these are all done (I used your sketch as a reference for which parts go "through" the other parts), you can create a Mirror, and Use a Boolean to join any parts that belong together:



Next, create a Circular Pattern:



The final Step is to do one last Boolean Union to combine all the parts that cross the original mirror planes. Since all the bodies are not touching anything else, you can use a Single Boolean Union feature, and it will combine all the touching bodies in a single feature. You could get real smart and do the Union before the Cicular Pattern - but I did the Pattern first in this case:


And that's it!


In many cases, complexity in sketches should be avoided, since Onshape has to work a lot harder to calculate and render all the sketch elements. Using Symmetry (both planar and rotational) and Boolean Operations can greatly simplify your work, the robustness of the model, and the "overhead" on Onshape's servers (and therefore the performance of your model as you continue to work on it).

Here's the link again to my public copy of your document: https://cad.onshape.com/documents/55b0a16cbce6cd863b66bb79/w/773f47e393e1cbb5488c13af/e/6fe7b1158e7a824400a93091

Hope this helps!
Good luck!

romeograham

Another point about this method: Now that you have a "solid" model that represents all the bodies and edges you want, you can use the faces of the parts to Extrude from or do other operations (rather than needing to extrude from a complex sketch).