Carmen, how about a single sketch mirrored about a centreline so an update to one half changes the other. Then 2 cut extrudes where you use the "Selected Contours" option to pick only one of the shapes. You'll have to expand Selected Contours within the property manager of the cut feature as it will default to being collapsed.
Repeat for the other side and use the same suppres/unsuppress technique.
An important and rather unknown part of that answer is that you can independently suppress features and their sketches. That means you can create multiple features from one sketch, or only suppress the feature so you can reference the sketch in other sketches.
It also explains why a 'feature' can give an error or warning even though it is suppressed. Because the underlying sketch is still unsuppressed and has an error.
I tried the following:
A mirrored sketch across centerline.
Then in Left config, select the left countour. Apply to "this config".
Then in Right config, select the other countour. Apply to "this config".
But it switched them both.
That leads me to believe that "Selected Contours" is not a configurable property.
Did I miss a step?
I think this is logged under SPR 365503 as it not respecting the config options. I think it may only respect the numeric inputs (depth and draft) and end condition. So two separate features may be needed.
Are those bodies mirrors of each other? It looks like they are. If that's the case, I'd model one, then create the second with the Mirror command. Next delete the body of the first one (Insert > Features > Delete/Keep Body). Now you have one body (the mirrored one). Suppress the Mirror and Delete Body feature in the other configuration, so you have the original body for your second configuration.
Thanks for the tip.
"Delete/Keep Body" is new to me. The trouble is that it either wants to delete everything or nothing.
When I try to follow your suggestion to "delete the body of the first one" using "(Insert > Features > Delete/Keep Body)", how do I select just the part I want to delete?
Here's what happened:
In a part file, I made a block.
Then I cut a hole in the block.
"Next delete the body of the first one (Insert > Features > Delete/Keep Body)."
I try to select the original cut-extrude by clicking in the hole shown by red arrow. But the entire block is selected, and it says that "mirror1" is selected. Anywhere I click on the part, it says "Mirror1" in "Bodies to delete"
I click accept and get a totally deleted part.
I select "Keep Bodies" and it keeps the whole thing.
I tried to extrude a block from the main block and had similar results. It's all or nothing.
I tried selecting the "Cut-Extrude" from the tree. It would not select.
How do I select "the body of the first one"?
What Adam Hartles said. Instead of mirroring the hole, mirror the entire body. I'd have a plane offset from the body so that the Mirror function creates two separate bodies.
So here's one configuration...
...and here's the other one...
That's brilliant, thanks!! I've got LH & RH configurations for seals and other flexible parts, and I was going nuts trying to figure out how to do it without remodeling each configuration. This is going into the company Solidworks Tips doc!!
I'm glad I could help.
Another way to mirror your part is to add the part to an assembly and mirror it in there (the advantage here is that it will create a new part automatically for you that is parametrically linked to the original part).
I was trying to create lh & rh models for a seal. They needed to have the same part number, so I to have the configurations in the same file.
Because SW 2017 has issues with using singular sketches for multiple features when selecting only some of the contours of the sketch used in individual features (such as what you have, 2 feature cut extrudes). The issue is that, if adjusting a parent item that the singular sketch is on (for a plane), the feature contour for each has to be re-selected.
1 sketch 2 individual cut extrudes
What you could do is create a base sketch of the cut-out geometry, sketching for both sides.
Create an individual sketch with converted geometry for each in each sketch. Then extrude cut each sketch as desired.
When you need to update, just update the base sketch and both will be updated.
Seen as 1 base sketch
2 individual sketches
2 individual cut extrudes
You could also create a base sketch of the cut-out geometry, sketching for both sides.
Create an individual sketch with converted geometry for one side, then extrude cut the one side from the individual sketch as desired.
Then mirror the cut extrude.
Seen as 1 Base sketch
1 individual sketch
1 individual cut extrude
1 mirror feature.