Hi Experts
INV 2020
How can I fill the space highlighted in the attached image 1 ?
I applied shell to make 2.5 thick material, how can I delete the high lighted portion in image 2.
Not sure which question should have been asked first, but hope my requirement is clear.
Part attached
Hi,
If I understand correctly you want it like this?
I added an extrusion between the sweep and shell command. You can see it in the attached ipt
I noticed you saved this as a sheetmetal part. Be aware this part will not create a flat pattern and is not strictly sheet metal.
Kind regards,
Alexander Boogaard
You just need to select the inner surface on the "Remove Faces" command. , is correct this is a stamp part.
Hi! Alexander is right. The reason why the sweep faces cannot be re-intersected is because of the type. The surface is spline-torus. The extension of the torus is going inward, not straight. In your case, the desirable extension is straight.
Unfortunately, Inventor is not that smart to tell straight is the desirable outcome. So, you need to provide the straight extrusion (Extrude or Thicken). After that, the faces can be re-intersected properly.
Many thanks!
Delete face worked.
@alexanderboogaard I understood the extrude feature way of doing this.
Just wondering is there any other approach of doing it in the model I have attached here to fill the void homogeneously. Extrude is giving a flat surface at the center.
I am looking for a shape like "A", at the moment we can acheive only shape "B".
@johnsonshiue Can you have a look why delete face (exactly the same thing you did) is not working in the attached model.
What is the significance of "thicken" here .
The delete face doesnt work "automatic blending"
Can I remove the highlighted lines that represents the shape transition from the attached model ?
Hi! "Auto-Blending" option operates more like Move Face or Extend. It tries to extend or contract the selected face and the adjacent faces re-intersect accordingly. The regular Thicken (Auto-Blending off) is offsetting. It protrude the face in the normal direction and the side faces are created accordingly.
In this case, the face is an ellipse. The extension will not be linear as you wish. As a result, it can fail on intersect.
Many thanks!
Hi! First of all, Inventor is not as smart as it seems. In this case, the side adjacent faces are ellipse. When you delete the planar face, the side elliptical faces will extend and re-intersect. However, there is no intersection with the extended ellipse.
I believe your design intent it to have the side faces extend linearly (tangentially). That is not how it works in this case. As a result, Thicken is needed here to provide the linear (tangential extension). After that, the Delete Face will work.
This is indeed a tricky case, because you will need to know how the faces intersect and how the Delete Face works.
Many thanks!
