is somebody sees why extending Surface-Offset B is possible, when trying to do the same with Surface-Offset H is not ?
Tx for your lighting.
Not without seeing what Surface-Offset B and Surface-Offset H look like.
Impossible to attach the file : i get always an error.
You've attached files before, haven't you?
What is the error?
How are you trying to attach the file? Are you using the Advanced Editor?
Even to reply here was impossible.
I erased all the cookies from SW, and now, it works .
I cross fingers
Always the same error.
Is there a way to know what are external relations, making impossible to move a sketch before another in the FM ?
Sure. Just Right Click on that sketch and select Parent/Child. On the left you get the parents, on the right you get the children.
Yes I did it.
Child/Parent says where are the endings of relations.
It would be very nice to have the extensive list of all external relations, if needed, yet.
Just try to flip a sketch, when there are some external relations, defined one month ago ...
At the first try I was able to extend 3 edges. The limitation is only in the geometry of the surface. It is not related in any way to the parent/child relationships.
See attached (I selected edges, not the face). If this is not acceptable for your purposes, let me know.
I found out why OffsetH cannot be extended on the 3rd edge. Follow this workflow for troubleshooting:
1. Rollback under Surface-Offset11 Feature
2. Copy the top face of the feature using an Offset zero command
3. Try to offset the newly created face by 12 mm.
4. You will see that one edge is curling in:
5. See attached.
6. That is why you cannot use that edge for offsetting only 2 mm.
Impossible to tag a "good answer".
Tx for your help
Hi Pet (or should it be Peever hum...)
The reason that you can not extend the surface H is because of th high rate of curvature at the end of Sketch 5 (see sketch 5.png below.) If you drag the tangency magnitude handle so that the curvature is more constant at the end (see sketch 5 corrected.png) then you can extend Surface H.
You might ask, what does that have to do with extend surface? Well, because the rate of curvature is really high (high rate of change) of the spline that created that surface - at that edge of the surface, extend surface has a tough time "quadratically extending (naturally extending.)
I noticed that you are extend linearly, but I believe you want to extend naturally, in that case, that is where this will be come an issue because the natural extension of that edge of the surface (because of the spline) can not extend that edge because it would loop back on itself.
Also, when creating spline profiles, you might want to try using as few spline points as possible and turning on "show curvature. See the difference between the your original sketch (original sketch 5.png) and the one I drew over it (redo of sketch 5 with fewer points.png) I did this with only with 5 spline points (verses your approximately 14) and because of this, you can get a much smoother curve.
Take a look at the following video for more: http://files.solidworks.com/special-videos/working-with-splines.zip
You are right : I would at first extend naturally, so quadratically.
Btw, I didn't understand naturally, but quadratically sounds better : I know what the programm is doing (or is assumed to do)
That didn't work, so i tried linearly.
I am trying to extend, because i want a surface cut which don't work.
I noticed that when cutting at the boundary of a surface, I got some - boring, really boring !!!! one more time - error : if the cutting tool (surface or curve) don't go throw the boundary, cutting not works. Incredible, but true.
Here, I wasted about 3 or 4 hours, changing just one dimension, in a part which looked not too bad, just a parameter I try to change, to see what will happens.
Some "face1", offsetted good, stays at the same place, because the "face1" was the "face1"in my previous geometry, and remains "face1" in the new one. The SW parametric touch !!!!
Btw, is there a way to put a point at a distance L of a spline ? No, I didn't find such feature.
I am amazing how teams of engineers can work with such program !!!!
Why all those offsetting and triming ? just for one reason : with SW a child surface kills a parent, when triming, cutting and so on ....
It was surely too complicate to have some option : "keep the parent feature", after any triming.
This file is unreadable, and I drawed it one week ago....
Is there a way to get curvature + normal vector at a given point ?
Working with osculating circles, perhaps i will modify this file more easily ....
Pet Peever wrote: Is there a way to get curvature + normal vector at a given point ? Working with osculating circles, perhaps i will modify this file more easily ....
Pet Peever wrote:
Have you considered using the Curvature tool? It will give you the curvature and the radius.
Watch this short video for a possible answer to your question.
Regarding getting the vector direction, you can just draw a line perpendicular at that point to the spline.
Tx a lot for your help.
I also searched how to get the normal vector (which is computed, since the curvature combs spread them).
But I didn't find how to get them.
Retrieving data ...