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.
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Alan
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Alan
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?
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JeffM
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.
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Alan
When I try that in the Config Manager, I just get the circle with the diagonal line indicating that I can’t do that.
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MarkKaiser
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.
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Alan
I’m running SW09SP2, and here is what I am trying,
Config A
Config A exploded
Config BWith Config A exploded open/active, lmb (or rmb) drag down to Config B, circle with diagonal line.
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MarkKaiser
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.
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Alan
I must have been moving my cursor too fast and didn’t see the left arrow. Thank you.
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Alan
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?
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MarkKaiser
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?
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Alan
The appearances in the display pane are all good. Per your suggestion I tried RMB and selected clear all top level overrides, nothing changed.
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MarkKaiser
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
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.
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Alan
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
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CBL
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?
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Alan
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.
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CBL
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?
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Alan
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.
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admin
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
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JeffM
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.
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CBL
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.
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Alan
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.
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Alan
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.
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admin
Cut revolve on a plane that is on the center axis of the shaft?
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Alan
I tried that, but it wanted to revolve around the shaft not my center line in the sketch.
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admin
Like this?
http://www.solidjott.com/wp-includes/images/Sketch.jpg
http://www.solidjott.com/wp-includes/images/Sketch02.jpgChoose 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
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
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gol10dr
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!
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sldprt
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.
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Alan
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.
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admin
Click “File-Save Sheet Format” is is a option just below the “Save As” on the file menu Unless you have tried that already
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Alan
That was it, I was thinking that the file save sheet format was a .drwdot file format.
Thanks
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Alan
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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CBL
Maybe this will help.
http://www.mitcalc.com/doc/tolerances/help/en/tolerancestxt.htm
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CBL
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Alan
Thank you CBL, those are great references. I was looking more at how this feature is used in SolidWorks.
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Chris Serran
The Fit Tolerances is for displaying tolerances on dimensions. It goes as far as showing how to apply predefined tolerances to a dimension.
You can use this when in the part or in the drawing to show a tolerance on a dimension.However, in order to analyze tolerances you need to use TolAnalyst which is only available in SolidWorks Premium.
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CBL
I believe Solid Professor had a video on this in their sample tutorials.
See the LMS download at http://www.solidprofessor.com/downloadlms.asp
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CBL
This is what I was thinking of, but it apparently access to the archive is not free.
See the last question at http://www.solidprofessor.com/asksp_archive.asp?page=2
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Alan, 
CBL, and 
MarkKaiser, and 
sldprt, 
Chris Serran, and 
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