Solidworks 2015
Close
Login to Your Account
Results 1 to 19 of 19

Thread: Solidworks 2015

  1. #1
    Join Date
    Jan 2018
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    1

    Question Solidworks 2015

    Hi, Everyone,

    I am trying to create a two roller mold/die that will mold a dough-like material. The problem I am having is that the border on the cavity has a twisted sweep in a arc. I need to inbed half of the sweep into one roller and the other half into the other roller so that each half is conformed to the cylindrical shape of the rollers. I tried to do this with the sheet metal tools by adding it in the flattened state, but when it is goes back to the normal form, I loose the cavity. I also tried to project the arc onto the roller and then do the sweep, but then it won't allow the twist. I am sure that this is possible in solidworks but have not been able to figure out how.

    Does anyone have any suggestions?

    Haroldforming-roller.jpg
    Last edited by Haroldana; 01-24-2018 at 01:54 PM. Reason: i don't know why is says plastic at the top of the post.

  2. Likes TopSolidCAM... liked this post
  3. #2
    Join Date
    Jun 2015
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    1,040
    Post Thanks / Like
    Likes (Given)
    239
    Likes (Received)
    545

    Default

    Really difficult to understand what is it that you trying to make. Some views could help. In general, you cannot use the flattened state in an assembly as it is only meant to fabricate the sheet metal.

  4. #3
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    402
    Post Thanks / Like
    Likes (Given)
    201
    Likes (Received)
    296

    Default

    Like Bill said, really hard to picture what you're trying to make or do without a visual aid.

  5. #4
    Join Date
    Apr 2013
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    753
    Post Thanks / Like
    Likes (Given)
    624
    Likes (Received)
    604

    Default

    Quote Originally Posted by Haroldana View Post

    Does anyone have any suggestions?

    Harold
    Pictures. Hand sketches. Anything.

    I have no freaking clue what you're trying to do.

  6. Likes BugRobotics liked this post
  7. #5
    Join Date
    Jan 2018
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    1

    Default

    Hey, Guys,

    Thanks for your comments. I updated the post with a picture of what I'm trying to do. The idea is to wrap and embed teh twisted ring shape into two opposing rollers and have them form the material by rolling them together.

    Thanks!

    Harold

  8. #6
    Join Date
    Aug 2010
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    52
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    40

    Default

    You want something like this?

    twistexample.jpg

    Create the roll, then define a sketch plane tangent to the roll surface. Sketch a circle on that plane then use the wrap to scribe it onto the roll surface. Then on a plane perpendicular to some part of the scribed circle sketch the profile you want to twist around. Perform a swept cut using the scribed guide as your path and the number of twists you want.

    Ignore the .zip file below. The .sldprt didn't upload properly because the size exceeded server limits and now I can't delete it.

    I'll host it for a few days for you to download if you want the example:
    TwistExample.SLDPRT


    Ivan
    Attached Files Attached Files
    Last edited by isvrcek; 01-24-2018 at 03:34 PM. Reason: .sldprt file not attached properly

  9. #7
    Join Date
    Jan 2018
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    1

    Default

    Thanks so much Johnny. I'll try this.

    I'll let you know how it works!

    Harold

  10. #8
    Join Date
    Jan 2018
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    1

    Default

    Hi, Johnny, and all,

    Does it matter if it is a circle or an arc? I tried it with a 180 degree arc and it will not work.

    Any comments will be appreciated.

    Thanks!

    Harold

  11. #9
    Join Date
    Jan 2018
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    1

    Default

    Hi, Johnny,all,

    I got it! It was because the contour must be closed. Once I closed it, it worked perfectly!

    Thanks so much!

    God bless all!

    Harold

  12. #10
    Join Date
    Aug 2010
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    52
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    40

    Default

    Where is it not working? The wrap function can throw an error if you don't have a closed sketch. You can solve that by drawing the arc you want and then closing it with another arc or line. Then just select the individual line you want for the sweep guide.

    I find the start and stop conditions of a swept cut are generally more troublesome so I would probably recommend doing the sweep for the whole circle then re-extruding or revolving your roll to cover the area you don't want back up.


    If the failure is in the swept cut operation you could have a problem with a zero thickness result or the sweep self intersecting.

  13. #11
    Join Date
    Aug 2010
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    52
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    40

    Default

    I see you found it!

  14. #12
    Join Date
    Jan 2018
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    1

    Default

    Hi, Everyone,

    I'm still working on this project and am having trouble getting the middle section(Area in Blue) hollowed out in a concave fashion twistexample.jpg. I want it to slope from the spiraled edge in a bowl shape toward the center of the circle. I have tried the Freeform command, Indent and the Deform commands, but they don't seem to work. The Freeform comes the closest, but disappears when I click OK. I'd greatly appreciate any help I could get!

    Please see attached Photo.

    Thanks,

    Harold

  15. #13
    Join Date
    Dec 2008
    Location
    tempe,arizona,usa
    Posts
    1,618
    Post Thanks / Like
    Likes (Given)
    132
    Likes (Received)
    178

    Default

    Quote Originally Posted by Haroldana View Post
    Hi, Everyone,

    I'm still working on this project and am having trouble getting the middle section(Area in Blue) hollowed out in a concave fashion twistexample.jpg. I want it to slope from the spiraled edge in a bowl shape toward the center of the circle. I have tried the Freeform command, Indent and the Deform commands, but they don't seem to work. The Freeform comes the closest, but disappears when I click OK. I'd greatly appreciate any help I could get!

    Please see attached Photo.

    Thanks,

    Harold
    Now this is a tough one with all thoughts tombstone edges wrapped around the cylinder and trying to make a smooth depression that is both going down and upwards as it transitions around the cylinder.

    can it be done? Well kind of, it will probably need to be done as a bunch of surfaces, planes and sketches to accomplish what you want.

    you'll have to explain to us how deep and what your think the shape should look like, make a hand sketch and scan or take a pic, put it up here and the let us digest it.

    you could put the model up here also or put a link to Dropbox, Google Drive or GrabCad for us to download to see what we could do. Most of us no longer are on SW2015 so the model will not be backwards compatible, we'd have to send you a parasolid for you to see.

    you could also get yourself a free version of Fusion 360 and the use the tsplines portion of it where it allows push pull of faces, might be the cat meow.

  16. #14
    Join Date
    Aug 2010
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    52
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    40

    Default

    What exactly is the shape you are shooting for? I don't have time to make a demo right now but I think a spherical depression (a spherical resulting part that is) could be done with a revolved cut on an axis perpendicular to, and offset from, the roll axis. Anything else though is probably difficult.

    Will there be any other geometry you want to add in? If so then it might be better to pursue making a macro. For example, create the desired final part and then use it to iterate a very large number of combine subtract cuts from the roll. This would have the benefit of allowing you to make rolls for any pattern you want easily after you made the macro.

  17. #15
    Join Date
    Aug 2010
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    52
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    40

    Default

    Quote Originally Posted by isvrcek View Post
    I think a spherical depression (a spherical resulting part that is) could be done with a revolved cut on an axis perpendicular to, and offset from, the roll axis.
    On second thought what I originally was thinking wouldn't be correct. You might not be able to tell the difference in practice but it wouldn't be right.

    You can make a true depression though with a swept solid cut. Sketch a circular sweep path that would cause a sphere that travels along to intersect the roll at the depth of depression that is desired.
    dishsketch.jpg

    Then revolve the sphere to make a solid body (do not merge).
    dishsphere.jpg

    Finally use the swept solid cut with the circular sweep sketch and the sphere body.
    dishresult.jpg

    I know the description is lacking. Hopefully the pictures get the idea across. If not here is a link to a sample file that I'll host for a few days.

    DishExample.SLDPRT

  18. #16
    Join Date
    Dec 2008
    Location
    tempe,arizona,usa
    Posts
    1,618
    Post Thanks / Like
    Likes (Given)
    132
    Likes (Received)
    178

    Default

    Quote Originally Posted by isvrcek View Post
    On second thought what I originally was thinking wouldn't be correct. You might not be able to tell the difference in practice but it wouldn't be right.

    You can make a true depression though with a swept solid cut. Sketch a circular sweep path that would cause a sphere that travels along to intersect the roll at the depth of depression that is desired.
    dishsketch.jpg

    Then revolve the sphere to make a solid body (do not merge).
    dishsphere.jpg

    Finally use the swept solid cut with the circular sweep sketch and the sphere body.
    dishresult.jpg

    I know the description is lacking. Hopefully the pictures get the idea across. If not here is a link to a sample file that I'll host for a few days.

    DishExample.SLDPRT
    problem is he needs the edges of the original cut and dimple from those edges.

  19. #17
    Join Date
    Aug 2010
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    52
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    40

    Default

    Quote Originally Posted by len_1962 View Post
    problem is he needs the edges of the original cut and dimple from those edges.
    I misunderstood then, what I showed will definitely remove the interior edges cut by the original sweep. The resulting rolls would not make two separate pieces.

    If the OPs intent though, as I originally read it, is to form a single piece lens shape with a twisted rope kind of border then this swept ball would do that.
    lens.jpg

  20. #18
    Join Date
    Aug 2010
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    52
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    40

    Default

    Quote Originally Posted by isvrcek View Post
    If so then it might be better to pursue making a macro.
    I forgot about the deform tool since I don't often use it but it is probably the simplest approach to all of this now that I think of it (that is when it works and doesn't error out).

    Create a solid of the molded part you want. I'll go with the lens and rope border I made in the last post. Then use it to make a combine subtract cut from a flat part that will become half of the roll.
    lenssubtract.jpg

    Then make two sketches. One with a line centered on the original part and longer than the flat part. The second will be an arc equal in length to the line. The radius of the arc is the radius of the desired roll. The midpoint of the arc should coincide with the midpoint of the straight line and tangent to it.

    deformguidecurve.jpg

    Then Insert > Features > Deform. Type: Curve to curve. First deform curve: the straight line sketch. Second curve: the arc segment sketch. Deform region: fixed edges yes, uniform yes, the body you created by the earlier subtract operation. Shape Options: Maintain boundary yes, match curve direction.

    curvedeform.jpg

    This result is actually probably more accurate than the swept cut I first proposed to give your border.

    curvedeformresult.jpg

    Like the other files. I'll host an example .SLDPRT for a few days in case the description isn't sufficient:

    DeformDemo.SLDPRT

    Ivan

  21. Likes len_1962 liked this post
  22. #19
    Join Date
    Jan 2018
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    1

    Default

    Thanks! Guys,

    Sorry for the tardy response. Very helpful!


Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •