I am having an issue supressing a single part as it seems to be supressing multiple parts at the same time?
Please see video attached for further details.
If a feature has any relations (colinear, coincident, are the common culprits for me) to a feature above in the feature tree, suppressing the top feature will suppress all of the features below. Right click on the feature and click "Parent/Child" to see what features are related.
Remove the relations and you will be able to suppress one without suppressing the other.
If you have any links to other features or common geometry it will suppress all the features that are inter-connected. If you right click on the part and go to parent/child it will tell you what other features are the child, and will therefore be suppressed as well. This happens a lot when your sketching and the automatic relations are used, you can link to something else and not even know it.
Easiest why to break the links is to go into the sketch and display relations, and use the drop down box to show external, these will be the relations to other features.
When you suppress the parent of the child, the child will suppress as well. You have features tied to the LOR revolve so when you turn it off, the children don't have anything to be built from.
I imagine the other features or their sketches have at least one relation to the feature, it's sketches, or the edges it creates. You'll need to free these relations in order to acheive what you're after.
If it's the sketch(es), you'll need to edit the sketch, delete any relations (dims included) to the geometry created by the feature in question. You'll want to add new dims to define the sketch.
If you've created the other features with relation to the feature in question (up to vertex for instance) you'll want to simplify that to a blind length.
This is probably the most difficult and overlooked in "Design Intent" - That is one of the benefits of using a Master Sketch, using a Master Sketch you can delete any feature or in assembly, any part without throwing errors...
I completely agree with design intent and master sketch.
However when dealing with others models and techniques I have found Dynamic Reference Visualization VERY helpful.
It gives me a quick visual parent/child reference. Saves lots of time hunting things down.
2015 SOLIDWORKS Help - Parent and Child Relations
Also another useful way of quickly finding where the relations start because it can be a chain of parent child relations. (you might be trying to suppress the great great grandparent) Is to try re-ordering the features in your tree and seeing how far an item can be dragged down or up the list and see where the first relation conflict takes place.
Generally speaking this entire situation can be avoided in the first place if all models are related in a logical manner so that items that are suppressed as it would be physically impossible to produce the 2nd feature without the 1st as a build material. Dimension based on design intent and not to just fully define the geometry.
Like I said above, these parent / child relationships between features happen most frequently due to automatic relationships in sketching. The best way to avoid them is to sketch so no relations happen and then lock the sketch into the main planes or a Master Sketch like John said. The automatic relations in sketches make it real handy, but when you got to rework something they can cause a headache.
What I would like to see is a way to unsupress parent and all children in one click.
Well, there kind of is a way....but its not one click. Its less than selecting the items one by one though:
Thank you Dan.
Or unsuppresse the lowest suppressed feature and all parents will unsuppresse
Doesn't work for me. See this movie I made...
Sorry, for not being abundantly clear that it only unsuppresse features with a parent relationship.
Rick, may I inquire why you are using a revolve cut for your 'slots' and not an extrude cut and a fillet on floor?
Jason, not much I can say to defend myself?
Because I can?
It's a feature damit?
Only the results count, not the journey?
Due to the many bugs and shortcomings, this is my workaround?
How about the truth.
This is a customer supplied file. I didn't model it. It just happened to be on my screen at the time so I used it instead of one of my Artwork pieces.
That is correct, but it is NOT the exact opposite of suppressing a parent and all children will suppress.
A feature has 4 children. Suppressing the parent will suppress all 4 children.
HOWEVER, unsuppressing one of the children will ONLY unsuppress the parent, and NOT the other children.
You can add them to a folder and suppress that.
I've done it myself just now,, here with an equation but same applies manual
You can always use shift to select a range of features or use Ctrl to select individual features one at a time, then suppress / unsuppress. Not quit 1 click, but still faster then doing them all one at a time.
When I want to have several features that I can suppress independently of each other I generally suppress each feature (or roll back above it )after I have made it before I make the next feature. This ensures you are not picking up unintended relationships. When you are done you should be able to pick and mix
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