In this part Mold Tool produced a distorted surface around this edge therefore I used non Mold Tool method. But the issue is I am unable to split the body into core and cavity. How to fix it?
In this part Mold Tool produced a distorted surface around this edge therefore I used non Mold Tool method. But the issue is I am unable to split the body into core and cavity. How to fix it?
Maha,
I think you are trying to "split with surface" feature and that 2 corners may not create a perfect edge
You have 2 options
Hope this helps
Is it possible to close gaps between solid and surface? because I found that it is gap creates split issue.
These corners are the problem edges.
You can extend the same surface out, then sweep.
Knit all together, then try split
(sorry, don't have 2019 so I viewed/exported via eDrawings)... this is a idea on how to do it another way..
Work is bit confusing to understand as it was viewed/exported via eDrawing. I have attached an original part file in a parasolid format. Repeat work is highly appreciated.
..sure, here it is..
Thanks. I am curious about to know how you use Surface Radiate tool as this tool is new to me.
Tooling Split produces error message. How to fix it?
..no idea why.
Maha,
I took a different approach and was able to use Mold Tools without problems.
1. I used your sketches to create 2 revolved surface bodies (Lower & Upper)
2. From the Top plane I used a circular sketch to extrude UP TO the lower surface. This allowed me to add Draft to the feature.
3. Used your Sketch3 to extrude UP TO the upper surface. Again I could add draft. And merge bodies.
4. Next I did the fillets.
5. Now I did the shell with bottom face open. This allows the fillets to show up on the inside.
6. Next I used your Skecth10 to cut the front opening. I made the top line coincident with inner top edge. This avoids that razor edge. Also we now have a good 1 mm corner radius. (No need for a separate Fillet feature.)
7. Next I did a 0 Surface Offset of the Inner face and front lip. (This will be needed later for the Parting Surface.)
8. I redid your 3DSketch5 to be a 2D sketch on Top plane. Now I could do an Extruded Cut with Outward Draft to get the top opening.
9. Then did a 3D sketch and converted the inner edges of the top opening. Used it to trim #7.
10. To clean up, I deleted the 2 revolved surface bodies.
11. Now I could Insert Mold Folders and do the Parting Line.
12. For the Parting Surface, I only used the edges that DID NOT define the upper opening. This allowed me to make the distance large enough (30 mm) to later draw a square to define Tooling Split.
13. I needed to do a Surface Fill to fill in the empty horizontal circular area..
14. Now I did a Surface Knit of the Parting Surface, Trimmed Surface and Surface Fill.
15. Last step was to do the Tooling Split.
Bill
Here is the core/cavity split using mold tools and surface tools combined
Mold tools will create the core/cavity split surfaces.
Parting surface is created using mold tools and surface tools
Thanks for the help.
I couldn't understand using Parting Line to trim the surface. It does not come to me. I trimmed this surface in a different way. File is attached
Maha,
That Trim Tool is not the actual Parting Line1 Curve, It's the Parting LIne1[3] cavity surface (that's showing highlighted)
Thanks, I got it. How to distinguish whether it is Parting Line1, Parting Line1[2] or Parting Line1[3] because in this box only it shows Parting Line1.
I am not sure how SolidWorks identify and pick the name
When you click on the selection box, particular area is highlighted in the graphics window
I don't know if there is a different way to identify the feature
Here's another approach. No surfaces required.
Please attach the file.
Here is the core/cavity split using mold tools and surface tools combined
Mold tools will create the core/cavity split surfaces.
Parting surface is created using mold tools and surface tools