Hello, I would like to fill the openings of this piece at the level of the curved shape.
Thank you for your help
image2.jpg
image2.jpg
Hello
I think an extrusion from the bottom of the opening to the surface won't work (but why not try).
We can then consider a scan with a normal sketch to the Z plane, then use one of the curves to serve as a guide curve.
I found the function I was looking for: "remove surfaces and fill in discontinuities":
To remove faces on a polygon body and fill in discontinuities:
1) Click Delete Face on the Surfaces toolbar or click Insert, Face, Delete.
The Delete Face PropertyManager appears.
2) In the graphics area, select the faces you want to remove.
The names of the faces appear in the Faces to Delete box .
3) Under Options, click Remove and Fill Gaps.
4) Click OK .
The faces disappear and the adjacent faces expand to form a surface without discontinuities.
See the image attached or on the help:
http://help.solidworks.com/2012/French/SolidWorks/sldworks/HIDD_DELETE_FACE.htm
EDIT: remember to also select the chamfers in the surfaces to be removed.
surface_combler_discontinuites.jpg
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Or do Insert/Face/Delete. Select ALL the faces to be deleted and confirm.
It also gives very good results.
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Hello
Have you tried in surfacics? Personally, that's what I would do:
- Offset of all interior surfaces to 0mm
- Restore surfaces to fill holes
- Then thicken to transform back into volume
What do you think?
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You can try a function recognition (if you have the possibility) only on the machining you want to remove.
For that you use the "featureworks" function with the "interactive recognition" option (or something like that)
You make him recognize the leave first and the removal of matter second.
If the function is not available:
You can do an extrusion from the inf face to plug the hole and then do a material removal by scanning to recreate the curved face.
There may be a solution by plugging the holes with surfaces and filling afterwards, but I don't know enough about the surface to tell you more.
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Hi @ g.becuwe
See this tutorial
http://www.lynkoa.com/tutos/3d/la-fonction-permettant-de-supprimer-la-face-dans-solidworks
@+ ;-)
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Hello;
Passes through the underside; Sketch it by collecting the edges (Convert Features icon).
Then extrude the matter to the curved surface, Merge your function well to have only one body.
To catch up with the chamfer of your rectangular shapes in my opinion only a sweep can do it, you will need the 3 seen with the hidden edges to better appreciate your problem.
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I would lean towards an extrusion from the underside of the part to the surface.
You may have to do it several times depending on the recognition of the surface(s).
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I have filled in the openings but now it has to follow the profile of the "curve" shape
Thank you for your answers
image3.jpg
_Esquisse to the middle plane of the form
_Sélectionnez the surfaces that make up the curved shape
_Ouitls/Sketching Tools/Intersection Curve
This gives you the profile
I have obtained an intersection curve, then what tools should I use to carry out a material removal following this curve?
Thank you for your answers
Insertion/Material Removal/Scanning.
Before you do this, you also need to have a sketch of the profile to scan.
@ benoit @ g.becuwe
I posted a tutorial
http://www.lynkoa.com/tutos/3d/la-fonction-permettant-de-supprimer-la-face-dans-solidworks
look it's super simple elementary
Delete and Fill function
@+ ;-)
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@GT22
It's super simple when the base file is clean. Otherwise it can quickly turn into putting a bandage on a wooden leg!
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@ g.becuwe
Is there a way to get the part?
The solution will be easier to find!
10 April, 2014 - 10:38 | /!\ Report abuse
@GT22
It's super simple when the base file is clean. Otherwise it can quickly turn into putting a bandage on a wooden leg!
In response to your answer, see the tutorial, the comments and you'll tell me
even if it's an imported comp it works
To try it and say what we think
@+ ;-)
Hello, I'm sorry, I had to put this piece aside for a little while.
So I'm coming back with the same part, but a guide curve that gives me an error with the scan function.
I thank you in advance for your answers and sorry again for the wait.
I also watched the video in tutorials, but on my piece I can't do it :-(
Kind regards
image11.jpg
Looking at your image, we can see that there is a surface body. And it suggests that this is your base volume.
I see that you have used the "Delete Faces" function. Have you checked the option "Delete and fill", "Delete and fill in gaps" or just "Delete"?
If you check this "Delete" option, your density body has become a polygon body (which I think since some edges have turned blue, a sign of a surface discontinuity).
If so, change this option (if the function wants to solve the surface!) and it will simplify your tree, or even save you from extrusions and sweeping!
If the "Delete face" function with the option "Delete and fill" or "Delete and fill discontinuities" doesn't want to work the first time, do it in 2 times starting by deleting the small leaves and then going through the pockets.
Finally, with your scan question, it may be that your profile (circle) crosses during the trajectory, let me explain: if your circle is for example 25mm in diameter, and your trajectory has a place with a retracted radius of 15mm for example, the top of your circle will cross :-/ So check the minimum radius of your trajectory.
If so, instead of a circle, draw a semicircle!
I don't know if you follow me?!?!
Good luck