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Question asked by Andrew Branch on Aug 6, 2020
Latest reply on Aug 14, 2020 by Tony Tieuli

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I'm working with a cylinder with hole configurations down the length of it. Is there a way to set up planes that always do a cross-sectional view of the holes? I want to cut the assembly in half and have the cut go along a plane that goes through the holes so I can present progress.

Currently, in an assembly I go to the sketch command and pick the feature I want to cut through and draw a line through it. Then I create a plane relative to that sketch and a parallel sketch face. What is wrong is that when I move the part the sketch stays in the same spot while the holes rotate of it. Is there a way to have the sketch stay with the holes? Or is there a better way? My way is a little time consuming and I was looking for a better way. Thanks.

Kevin Chandler Aug 6, 2020 8:01 AM

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Hello,

Relocate your first part in the assembly so it's centered on the origin

Turn on view temp axes and mate a hole's axis to the right or top plane.

Repeat for each part. Currently, each is free to spin out of hole alignment.

Your part and assembly don't have any configs that you mentioned in the OP.

Kevin

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Dario Karalic Aug 6, 2020 7:00 AM
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I cant open your files because they are future files for me. When you create sketch in assembly (i assume you draw line from one circle quadrant to another and make plane (section there) . If sketch stays at same spot when you move component did you try to force rebuild it (CTRL+Q) ?
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- Andrew Branch @ Dario Karalic on Aug 6, 2020 11:26 AM
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  @Dario Karalic I don't know why my file wouldn't work but there are lots of pay walls.
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Kevin Chandler Aug 6, 2020 8:01 AM
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Hello,

Relocate your first part in the assembly so it's centered on the origin
Turn on view temp axes and mate a hole's axis to the right or top plane.
Repeat for each part. Currently, each is free to spin out of hole alignment.

Your part and assembly don't have any configs that you mentioned in the OP.

Kevin
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- Andrew Branch @ Kevin Chandler on Aug 6, 2020 11:23 AM
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  Kevin Chandler I'm not sure how to "relocate your first part in the assembly so it's centered on the origin"
  I've just recently learned you can orient to the datums in assembly. I get how to insert a part normal to a plane only when I newly add it to an assembly. I insert the part and as it is following the cursor, I change the view to the front plane to place all parts because that's the best I could figure out on my own.
  
  Could you give any steps to having a badly oriented part (like when you lose it into space randomly) moved back to the view panel and what commands you call up (with drop down menus? or right click?). I haven't been taught many of the amazing glitches I've seen and deal with on a regular basis. I know about the quick menu "last view" command and that has helped me out of a lot of mistakes.
  
  I know that you can line the parts up by fixing them in place but I meant is there a way to save a configuration. Like I've been thinking for meetings it would be good to have written several orientations and be able to quickly move through them while explaining in words what is going on. I'm looking for steps to orient so I can practice.
  
  Thanks for replying and I will take what I can get because I love working with CAD software.
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  - Kevin Chandler @ Andrew Branch on Aug 6, 2020 12:17 PM
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    Andrew Branch wrote:
    
    Kevin Chandler I'm not sure how to "relocate your first part in the assembly so it's centered on the origin"
    I've just recently learned you can orient to the datums in assembly. I get how to insert a part normal to a plane only when I newly add it to an assembly. I insert the part and as it is following the cursor, I change the view to the front plane to place all parts because that's the best I could figure out on my own.
    
    Could you give any steps to having a badly oriented part (like when you lose it into space randomly) moved back to the view panel and what commands you call up (with drop down menus? or right click?). I haven't been taught many of the amazing glitches I've seen and deal with on a regular basis. I know about the quick menu "last view" command and that has helped me out of a lot of mistakes.
    
    I know that you can line the parts up by fixing them in place but I meant is there a way to save a configuration. Like I've been thinking for meetings it would be good to have written several orientations and be able to quickly move through them while explaining in words what is going on. I'm looking for steps to orient so I can practice.
    
    Thanks for replying and I will take what I can get because I love working with CAD software.
    Hello,
    
    First suppress all of the mates for the first part (usually, but your mates won't restrict the required movement).
    Right click the first part in the tree and select Float (the fixed "F" is now gone).
    Select the Top plane of the assembly and the Top plane of the first part and add a coincident mate:
    Repeat this for the right planes. And then the front planes.
    The part is now aligned to the assembly planes.
    Delete the 3 coincident mates you just created and right-click the part in the tree and select Fix (the fixed "F" is now back).
    Unsuppress the the original mates.
    
    Add a concentric mate for each part, to the same hole on the first part.
    
    Kevin
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    - Jeremiah Feist @ Kevin Chandler on Aug 6, 2020 5:28 PM
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      instead of mating the 3 planes, add a coincident mate between the part origin and assembly origin - it will default to "align axis".
      
      also. not much point in suppressing the new mate(s) and re-fixing the part.
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    - Andrew Branch @ Kevin Chandler on Aug 14, 2020 4:35 AM
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      I forgot you could reference the datams on the part itself in the tree. Very helpful. Thanks Kevin Chandler
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- Andrew Branch @ Kevin Chandler on Aug 14, 2020 4:28 AM
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  This is something I didn't know I could do. Now I run into the problem that I can't render a cut through. I found a solution that I have to toggle on "graphic-only section" in the section view action panel when I use the plane orient method.
  
  To the overall discussion, I'm looking to orient and save certain configurations so I can create and save them to move through them quickly in a design meeting. Any tips that you have for quickly orienting and "saving" a spot that is cut through to see more of the assembly. I learned you can sketch in assembly and then make a plane normal to that sketch, usually just a line drawn on any surface in the assembly. Then if you select the plane and then immediately select section view, it does a cut through of that saved plane relative to the sketch. The only problem is if you don't fix your assembly in one place the sketch moves with the part you referenced for the sketch so you need to reference the sketch to a fixed spot. You could make several sketches and create several planes and then cycle through them 1 by 1 with the section view to move through several important features.
  
  I need help on defining an assembly to the origin I suppose, and figuring out what part of an assembly should be fixed. It's more a theoretical problem on your philosophy on how to solve a problem statement with an assembly.
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  - Kevin Chandler @ Andrew Branch on Aug 14, 2020 8:16 AM
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    Andrew Branch wrote:
    
    This is something I didn't know I could do. Now I run into the problem that I can't render a cut through. I found a solution that I have to toggle on "graphic-only section" in the section view action panel when I use the plane orient method.
    
    To the overall discussion, I'm looking to orient and save certain configurations so I can create and save them to move through them quickly in a design meeting. Any tips that you have for quickly orienting and "saving" a spot that is cut through to see more of the assembly. I learned you can sketch in assembly and then make a plane normal to that sketch, usually just a line drawn on any surface in the assembly. Then if you select the plane and then immediately select section view, it does a cut through of that saved plane relative to the sketch. The only problem is if you don't fix your assembly in one place the sketch moves with the part you referenced for the sketch so you need to reference the sketch to a fixed spot. You could make several sketches and create several planes and then cycle through them 1 by 1 with the section view to move through several important features.
    
    I need help on defining an assembly to the origin I suppose, and figuring out what part of an assembly should be fixed. It's more a theoretical problem on your philosophy on how to solve a problem statement with an assembly.
    Hello,
    
    One way is to save section views within the assembly without having to cut anything is to use saved section views:
    Create a section view and then scroll down and click Save:
    
    Give it a name:
    Tap Spacebar and the saved section views (as well as other custom views and the std ones) are listed:
    
    Selecting a saved section view turns on section view for you, but if you later select a std view or non-sectioned custom view, you must turn off section view yourself.
    
    Note: SW defaults to "SectionView" in the Save As box (I added 1, 2, 3), but SW appends a serialized index to "SectionView" (for automated view name uniqueness) and then it appended the number I typed.
    
    Note 2: If you also check "Drawing annotation view", you can drag the section view onto the drawing from the view palette. It will still be saved in the Orientation dialog.
    
    Kevin
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    - Tony Tieuli @ Kevin Chandler on Aug 14, 2020 11:06 AM
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      Kevin Chandler wrote:
      
      Andrew Branch wrote:
      
      This is something I didn't know I could do. Now I run into the problem that I can't render a cut through. I found a solution that I have to toggle on "graphic-only section" in the section view action panel when I use the plane orient method.
      
      To the overall discussion, I'm looking to orient and save certain configurations so I can create and save them to move through them quickly in a design meeting. Any tips that you have for quickly orienting and "saving" a spot that is cut through to see more of the assembly. I learned you can sketch in assembly and then make a plane normal to that sketch, usually just a line drawn on any surface in the assembly. Then if you select the plane and then immediately select section view, it does a cut through of that saved plane relative to the sketch. The only problem is if you don't fix your assembly in one place the sketch moves with the part you referenced for the sketch so you need to reference the sketch to a fixed spot. You could make several sketches and create several planes and then cycle through them 1 by 1 with the section view to move through several important features.
      
      I need help on defining an assembly to the origin I suppose, and figuring out what part of an assembly should be fixed. It's more a theoretical problem on your philosophy on how to solve a problem statement with an assembly.
      Hello,
      
      One way is to save section views within the assembly without having to cut anything is to use saved section views:
      Create a section view and then scroll down and click Save:
      
      Give it a name:
      Tap Spacebar and the saved section views (as well as other custom views and the std ones) are listed:
      
      Selecting a saved section view turns on section view for you, but if you later select a std view or non-sectioned custom view, you must turn off section view yourself.
      
      Note: SW defaults to "SectionView" in the Save As box (I added 1, 2, 3), but SW appends a serialized index to "SectionView" (for automated view name uniqueness) and then it appended the number I typed.
      
      Note 2: If you also check "Drawing annotation view", you can drag the section view onto the drawing from the view palette. It will still be saved in the Orientation dialog.
      
      Kevin
      It's amazing how many tips you can pick up browsing this forum.
      It never occurred to me to save a section view. I can't count the number of times I've opened and closed the same section view in one session! Such a simple thing and yet....
      Thanks Kevin Chandler!
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Dan Pihlaja Aug 6, 2020 4:59 PM
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Yes, you can do this easily:

You can create a plane at the part level and use that at the assembly level to either make an actual cut or use it for a section view:

1) At the part level Show your sketch:

2) Create your plane:

Notice that I have used the front face to be perpendicular to, and the two center points of the holes to drive the location of the plane.

Now I can use that plane to either create a section view OR drive an actual cut on the part.

And when I move the location of the sketches, the plane moves automatically.
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- Andrew Branch @ Dan Pihlaja on Aug 14, 2020 4:32 AM
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  This is also very helpful. I'm learning you can sketch just about anywhere. Most people want you to hide the sketches but I find them helpful to fix presentation issues. I already noted someone else as a solution but I like that you included screenshots; very helpful. Thanks. Dan Pihlaja
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