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  • Alan 10:13 am on March 2, 2009 Permalink | Log in to leave a Comment  

    I have a 3/8″ aluminum plate that has machined pockets on both sides. In my drawings, the isometric view will show (and print) 2 edges from the pockets on the back side of the plate when at zoom to fit, but when I zoom in to the area it will show correctly. Is there a way to eliminate these edges when printed? Right clicking and selecting hide edges is not an option since there is no real edge there.

     
    • admin 11:59 am on March 2, 2009 Permalink

      Can you attach a drawing and a part so that we can see this?

    • CBL 1:37 pm on March 2, 2009 Permalink

      SW has had a problem with edges bleeding through thin sections forever. It is usually seen in sheet metal parts.

      As a workaround, could you create a config with the underside pocket suppressed, and use that in the isometric?

    • Alan 6:53 am on March 3, 2009 Permalink

      This isn’t the first time I have seen it either, supressing the back side pockets is what I will have to do to avoid confusion by others looking at the drawings. Thanks

  • Alan 12:16 pm on February 2, 2009 Permalink | Log in to leave a Comment
    Tags: , ,   

    I have several assemblies with two configurations. The only difference between the two configurations is that there are a few parts with a different configuration. Is there a way to apply the same exploded view to the second assembly without having to do it manually a second time?

     
    • JeffM 12:31 pm on February 2, 2009 Permalink

      If I remember correctly, you should be able to drag/drop the first exploded view into the second configuration. Naturally you’ll end up with some errors, but it should be quicker.

    • Alan 1:34 pm on February 2, 2009 Permalink

      When I try that in the Config Manager, I just get the circle with the diagonal line indicating that I can’t do that.

    • MarkKaiser 1:50 pm on February 2, 2009 Permalink

      It’s just finicky. Try dragging the exploded view above the config name you want to copy to, that’s how it’s working for me in 09. You need to have the config active that you are copying the exploded view from also.

    • Alan 2:18 pm on February 2, 2009 Permalink

      I’m running SW09SP2, and here is what I am trying,

      Config A
      Config A exploded
      Config B

      With Config A exploded open/active, lmb (or rmb) drag down to Config B, circle with diagonal line.

    • MarkKaiser 3:01 pm on February 2, 2009 Permalink

      Alan,

      I’m not sure why it isn’t working for you. I get the circle with diagonal line, then when I drag it somewhere it can copy, it changes to a down and to the left arrow with a small plus sign next to it. Then it copies. If you’re dragging down (in the config tree), it may look like it’s dropping another copy under the active config, but it’s actually dropping a copy under the config below it.

    • Alan 6:49 am on February 3, 2009 Permalink

      I must have been moving my cursor too fast and didn’t see the left arrow. Thank you.

  • Alan 12:13 pm on January 26, 2009 Permalink | Log in to leave a Comment
    Tags:   

    I have been working on an assembly all day and having SW crash several times with errors indicating out of memory. This last time it shut down there was no error indication. When I re-opened the assy file, it had an appearance on it that I had not given to it. Watching the screen as it opens, it initially looks correct, but when it finishes building the appearance is applied. When opening up the sub-assemblies there are no appearances. I am unable to find where this appearance is comming from, how do I remove this appearance from the top level assembly?

     
    • MarkKaiser 12:29 pm on January 26, 2009 Permalink

      When you expand the display pane on the feature manager do you see any appearances out of the ordinary? If you RMB in the display pane, you get a clear all top level overrides selection, possibly this would fix it?

    • Alan 1:15 pm on January 26, 2009 Permalink

      The appearances in the display pane are all good. Per your suggestion I tried RMB and selected clear all top level overrides, nothing changed.

    • MarkKaiser 1:38 pm on January 26, 2009 Permalink

      Did you read the comments under Guido’s post two posts earlier than your’s? Sounds like he had a similar issue.
      http://solidjott.com/2009/01/23/i-have-a-couple-of-files-that-were-made/#comments

    • admin 1:54 pm on January 26, 2009 Permalink

      Mark, Alan we have come to figure out that it was most likely the hardware in Guido’s problem. I am not sure this is the case here.

    • Alan 2:04 pm on January 26, 2009 Permalink

      I just got off the phone with my VAR, somehow when my system crashed it turned all the files in that assembly to a default view that was not shaded with edges. After re-setting all those files and cleaning up my temp folder it looks good.

      Thanks

    • CBL 2:05 pm on January 26, 2009 Permalink

      If a crash was involved, the file could have become corrupted.

      Can you ask your VAR to take a look?

      If it’s not too big or top-secret, could you zip (Pack and Go) and post the files involved here?

  • Alan 1:48 pm on January 21, 2009 Permalink | Log in to leave a Comment
    Tags: , exploded views,   

    In an assembly I created a sub-assembly. In this sub-assembly I have a plate with components on both sides. I have saved this sub-assembly outside of the original assembly so that I can create an exploded view for a drawing.

    I would like to have a front and back configuration to have exploded drawings of each side. For the front config I have everything mated properly, but when I try to change the mates for the back config, the front config will then use the back config mates.

    What I am trying to accomplish is to have the front view aligned with the origin, and the back 180deg about the right plane.

     
    • CBL 5:37 pm on January 21, 2009 Permalink

      I don’t think I’m fully understanding the problem.

      You don’t need to change mates in order to create exploded views.

      Can you post images or the zipped assy?

    • Alan 6:55 am on January 22, 2009 Permalink

      I want to be able to have nice isometric views of the front and back of the plate for the drawings. With 2 configurations I would be able to have 2 seperate exploded views, one for the front side, and one for the back side.

    • admin 8:08 am on January 22, 2009 Permalink

      Ahhhh I think I see what is going on here. You do not have to re-create the mates and make configs to get a backwards iso view you can just make new iso angles with this macro and change the view in the drawing to one of the newly created views from the macro…

      http://sw.fcsuper.com/index.php?name=UpDownload&req=viewdownloaddetails&lid=62

    • JeffM 8:14 am on January 22, 2009 Permalink

      Instead of creating different configs, just create an “opposite iso” view. Start with your back view. Hit the space bar single click on ‘Front’. Click on ‘Update standard view’. Double-click on ‘Iso’ view. Click on new view and name the current view “Reverse ISO”. Click on reset standard views. Now, you’ll have your normal views plus your new view.

    • CBL 10:47 am on January 22, 2009 Permalink

      I understand now. Yes, you will need to create another config to be able to create a separate Explode under each. But you do not need to create new mates just to rotate the assy; The methods Ben and Jeff suggest will create the views which can be called into the drawing. The config can then be specified for that view.

    • Alan 12:21 pm on January 22, 2009 Permalink

      Thanks Jeff, this did work, and I still had to create a new config in order to create a different explode off of the back.

  • Alan 7:58 am on December 31, 2008 Permalink | Log in to leave a Comment  

    What is the best way to put a spherical cut on a side of a shaft? I have a .375 dia shaft that needs a spherical dimple on its side by use of a .125 Ball E’Mill to a depth of .030. All ideas appreciated.

     
    • admin 8:04 am on December 31, 2008 Permalink

      Cut revolve on a plane that is on the center axis of the shaft?

    • Alan 8:50 am on December 31, 2008 Permalink

      I tried that, but it wanted to revolve around the shaft not my center line in the sketch.

    • admin 8:54 am on December 31, 2008 Permalink

      Like this?
      http://www.solidjott.com/wp-includes/images/Sketch.jpg
      http://www.solidjott.com/wp-includes/images/Sketch02.jpg

      Choose the line to revolve about here by selecting the feild and then clicking on the revolve axis you want
      http://www.solidjott.com/wp-includes/images/2008-12-31_0902.png

    • sldprt 9:01 am on December 31, 2008 Permalink

      From your description, sounds like you are modeling this shaft inplace of your assembly. I would not recomend inplace modeling in most places. the origin, front, top, and right side place should make sense after open the part in its own window. then the shaft centerline should flow through origin. at that point you can establish an axis very easy.

      if this is not possible as you are too far into the modeling process, you can also show the shafts own axis of its faces. to do this goto view drop down menu and click show temparary axis. then use the axis localy in the part to establish a plane.

      hope this helps

    • gol10dr 11:06 am on December 31, 2008 Permalink

      You can also build the sphere body and use the combine command in the part to subtract it. I think the revolve cut is a better option and you may just need to adjust your axis selection that was mentioned!

    • sldprt 12:08 pm on December 31, 2008 Permalink

      I will also mention for interest reasons that you can sweep cut a solid body. Meaning that you can use a solid body as a profile for a cut, and have it follow a sweep path. This is good if you want to model your end mill and plot the path it should follow during the cut. This feature is in 2008 and later.

  • Alan 3:51 pm on December 15, 2008 Permalink | Log in to leave a Comment  

    Recently I tried to add a second sheet to a drawing, ans SW is looking for a .slddrt or .drt file which does not exist on my pc. I tried to do a save as to create this file type, but there are no options to save as a .slddrt or .drt file. Any ideas on how to resolve this would be appreciated.

     
    • admin 3:58 pm on December 15, 2008 Permalink

      Click “File-Save Sheet Format” is is a option just below the “Save As” on the file menu Unless you have tried that already

    • Alan 12:00 pm on December 16, 2008 Permalink

      That was it, I was thinking that the file save sheet format was a .drwdot file format.

      Thanks

  • Alan 6:19 pm on December 3, 2008 Permalink | Log in to leave a Comment
    Tags: Fit Tolerences   

    I was looking for something in SW help, and I ran accross a section on Fit Tolerences. I could really use this but the help section really didn’t explain enough for me. If someone could give me a better overview of this feature I would appreciate it. Thanks

     
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