Editing a sketch makes features disappear
When we edit a feature from the timeline, All the features after the edited features will be suppressed, its expected behaviour.
Could you please explain in detail about what the problem you are facing?
There are 6 holes on 3 faces, point them which hole has to me move by a mm. there will be multiple ways to handle a situation.
This Sketch10 is a little strange.
First of all, it is irregular to draw a sketch of a hole horizontally to a flat surface.
And it is also odd to have the dimensions at an angle.
Normally, you should draw the sketch on the plane on which you want to draw the sketch and put in the dimensions.
For example, like this.
That way, nothing will collapse if this 13 dimension is changed to 12 or 11.
I have attached the corrected file.
If the corrections are off the mark or if other corrections are needed, please ask additional questions.
@wcarlsonM2NUS , Sorry and @laughingcreek Thank you.
That expression of mine does not convey the intent, I am sorry.
"Usually, you draw a sketch on a plane with the same orientation as the direction you want to extrude and fill in the dimensions." I have rewritten it as.
The Sketch10 in the problem is drawn in the XY plane, so it should be pushed out to the Z axis.
The hole you are trying to make needs to be extruded in the x-axis direction, so it is usually written in the yz-plane. (See. Sketch16)
This time, however, for clarity, we indicate the plane near where the hole will be made.
The reason why such irregular sketches are possible is that this 3D Sketch is checked.
It is better to turn this switch on only in special 3D situations.
@wcarlsonM2NUS wrote:
...I don't understand sketchs 2 and 3. I don't see how they relate to the rest of the sketch...
sketches are related/linked to each other with projections from previous sketches (purple articles.) projections are one of the most important tools to use with sketches. if your not using them now is the time to study up. there are several types, and they are all useful.
turn on the visibility for dimensions for all there sketches so your screen looks like this-
DOUBLE CLICK on one of the DIMENSIONS, such as the one I have circled, and change it to a reasonable value. what do you observe? play around with all the dims and see what happens.
all the extrudes reference sketch articles using the START and EXTENT TYPE inputs in the extrude commands. the result is that you can look at the model like in the pic above to make adjustments instead of digging around in features in the timeline, which gets increasingly difficult as projects get bigger.
...I see you created half the sketch and then mirrored it for symmetricity. Ordinarily this would be great, but the holes on the other lug don't match.
then don't create holes that aren't mirrored till after the mirror feature. put them in a sketch and extrude/cut after in the same way the other sketches and extrudes where made.
You can use the sketches already created, or create new ones. I would still group sketches at the beginning of the timeline, and I would still put them on origin planes and not the faces of the solid.
@wcarlsonM2NUS wrote:
So sketch number 3 creates both lugs and a single set of holes that go through both lugs?
currently, yes. I had assumed a symmetrical layout of holes. you can just do the lug without the holes by adding the profiles of the holes to the EXTRUDE2 feature.
