Solidworks mold tool for a B pillar trim. 3

[Leeroy605]

Hello

I'm trying to created a mold tool for a B pillar trim. The part was made in Catia V5 and imported into solidworks using the IGLES file type then saved as a solidworks file. I've followed the tutorial in solidworks exactly but however when I go to create a tooling split I get the message "Cannot knit sheets together". Does anyone have any clues as to what I am doing wrong? I have attached the part below

Thank you

 

[kellnerp]

First of all, don't post sldprt files. They are not compatible with all versions of SolidWorks. People here run anything from 2009 to 2012. png, pdf or jpg is better for this kind of thing.

Second, when you bring in any IGES file you have to run it through IMport Diagnostics with TOOLS/OPTIONS/SYSTEM/PERFORMANCE stringent geometry checks turned on. You also have to check it with TOOLS/CHECK with surfaces and solid bodies turned on. If you get past all that on a solid body with a clean bill of health then try making the mold cavity.

TOP
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[CorBlimeyLimey]

First of all, don't post sldprt files.

I strongly disagree. While a picture speaks a thousand words, a solid model speaks the complete book. Most times a solid model is the only way to see what settings or techniques have been (mis)used, without wasting time playing the 20 questions game.

Post whatever SW format files you have for those who do have compatible SW versions, but parasolids and images would also be helpful for those who are not so fortunate.

 

[AnnaWood]

I agree with CBL....

Post your part files Leeroy605. There are plenty of us with the appropriate version of SolidWorks to be able to read your file.

Being able to see your specific modeling techniques will aid tremendously in us being able to help you out.

Cheers,



Anna Wood
SW2011 SP5, Windows 7 x64

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[Leeroy605]

Thank you for the replies

Interesting thoughts on the uploading debate, I would have thought the actual part would be much more useful as people can load it up and poke around to see what I'm doing wrong. I did not know some sldprt files were incompatible with other versions of solidworks.

Using the import diagnostics tool did come up with some errors which were due to the way it was made in catia, these have been rectified and the process leading up to the tooling split is much improved, however when creating the tooling split I still get the message about not being able to knit the sheets together.

I have included two versions of the updated part below, one with nothing done onto it and another with draft angles, scale, a parting line and shut off surface included. If any other file types are required let me know.

Again thank you for the responses.

 

[kellnerp]

Since this is an import problem, having the sldprt files is next to useless. The IGES file would have been more helpful. Many companies load the most recent SolidWorks a year or more later than the current release. So if you want the most people to look at your problem post a neutral file or picture.

At any rate what happened when you checked the model? What were the errors and what errors remain?

TOP
CSWP, BSSE

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Phenom IIx6 1100T = 8GB = FX1400 = XP64SP2 = SW2009SP3
"Node news is good news."

 

[Leeroy605]

Right ok the IGES file is attached below. After import diagnostics no faulty gaps or faces are detected, and the feature recognition comes up with an unrecognised body, holes 1 & 2 and four Varfillets. One of the varfillets comes up with an error once the feature recognition is completed but the position of it is way off the model below it, deleting it has no effect.

Are you positive this is an import error and not something I am doing wrong in the mold making process?

 

[kellnerp]

I had no problem creating a mold cavity. The IGES came in cleaner than I have seen in a long time.

The INSERT/FEATURE/CAVITY worked flawlessly.

Here is what I got: CAVITY

TOP
CSWP, BSSE

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[kellnerp]

I had to step away from my machine for a while. But I didn't have any problem generating a ruled surface for splitting the mold along one of the longer edges. If it goes as fast as the first ruled surface should take about 15 minutes to split the cavity.

I used ruled surface normal to vector and picked one of the edges of the mold as the vector.

Can you identify the area on the model where the problem occurred?

TOP
CSWP, BSSE

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Phenom IIx6 1100T = 8GB = FX1400 = XP64SP2 = SW2009SP3
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[Leeroy605]

I cannot as it doesn't give me a specific area, just that it cannot knit the sheets together however I don't quite fully understand what this means.

I cannot insert the cavity in the way you can, when I go to insert/feature/cavity the option is greyed out, and I have no experience using the ruled surface function. I guess you can tell how new I am to solidworks, if this was in CATIA it would be no problem!

The way I am trying to create a mold with the cavity and core is by following the inbuilt tutorials in the help section on mold design, which uses a model telephone. This is exactly how I want my part to come out but even following the exact same steps it's the tooling split part that won't work.

I thank you for taking the time to respond to my problem however, it really is appreciated.

 

[kellnerp]

Here is the complete split mold. SPLIT

To get to this point:
1. Create an assembly
2. Place the B Pillar into the assembly with appropriate mates
3. Create a new part in the assembly.
4. With the new part active, extrude a block of material around the B Pillar and insert a cavity feature. Hide the B-Pillar after making the cavity.
5. In wireframe display pick the appropriate edges of the B Pillar and create a swept ruled surface using the block edges for reference. See help on ruled surfaces.
6. Create four boundary surfaces to connect the four ruled surfaces. see help on Boundary surfaces (they are better than lofts for this.
7. Create three fill surfaces with merge turned on to fill the holes in the B Pillar
8. Knit all the surfaces. see help on knit
9. Insert a split feature and keep both bodies. see help on split feature.

This is all done while editing the block you created inside the assembly. The block should be blue in the feature tree. see help for editing parts in-context in assemblies.

The insert cavity feature will not work if you are not editing the part/block inside the assembly.

Help is your friend. I have given you the roadmap.

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

http://www.linkedin.com/in/engineeringtransport

Phenom IIx6 1100T = 8GB = FX1400 = XP64SP2 = SW2009SP3
"Node news is good news."