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Struggling with assembly configuration for controlling drawing views

Question asked by Murray Edington on Nov 21, 2015
Latest reply on Nov 29, 2015 by Murray Edington

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I'm trying to create a set of drawings, each sheet showing an a hydraulic ram assembly in a different position. I've tried to create a set of configurations within the assembly, one for each position, so I can call each up as required to show the piston in different positions.

I was expecting to find a "configurations" rollout offering "this configuration"/"all configurations"/"specify configurations" radio buttons, at which point I'd select "this configuration". But I can't see those choices anywhere. I seem to have created the configurations and can activate each in turn but they don't cause the assembly to reconfigure and the bottom line is that although I call them up as configurations within my drawings, they all show the assembly in the last state I left it in. It looks as if I'm changing all of the configurations when I change the mate distance, despite apparently activating a different config in each case.

If I understood the various references correctly (the SW help, Solidworks for Beginners, The Solidworks Bible, Youtube guides etc), I would create a new configuration ("add configuration"), make the changes (change a mate distance in this case) then save the assembly again. I would do this for each new configuration, ending up with 3 configs in my case. Then, when I wanted to show the piston in one of those positions in a drawing view, I'd call the right configuration up in the drawing properties.I seem to have done all that but still no cigar.

Can anyone suggest where I am going wrong here? It feels as if it's one of those simple problems that's staring me in the face but I can't see it. It may be that the critical controls have been moved in recent releases - I'm using 2014.

I tried a really simple assembly (a nut and bolt) with just 2 mates (concentric and distance) and I still have the same problem.

Mark Kaiser Nov 25, 2015 8:51 AM

Correct Answer

I second Craig. It worked for me, but I had to unsupress the distance mate in a couple configs also.

One thing to help might be what faces you are mating to, and if the distance mate dimension is required to 'flip' between configurations (change its direction). This might cause issues.

With the mate being suppressed, maybe this is the only problem, and when you are adding new configs, it is auto suppressing for you. Here are some pics to check that.

Distance mate showing suppressed when I opened your assembly.

RMB on config, click on properties.

Make sure checkbox 'suppress new features and mates' is not checked. If you create the mate first, then add configs, this box will mess with you. Do not remember if it is a system/document option somewhere, this box for me is always unchecked.

See the reply in context

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Glenn Schroeder Nov 22, 2015 12:05 PM

Find the distance mate in the tree. Click on it (or double-click, depending on whether or not you have Dynamic Highlight turned on) to show the mate dimension in the graphics area. Right-click on it and choose "configure dimension" from the drop-down. That will open a simplified design table with a row for each configuration and a column for the mate dimension. Enter the desired value for each configuration in the appropriate cell. If you want, you can name and save the table near the bottom of the dialog box for future editing, but the changes will take effect even if you don't.

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Murray Edington @ Glenn Schroeder on Nov 24, 2015 7:17 AM

Thanks Glenn - that seems to be heading in the right direction, although I'm not out of the woods yet.

The reason for the delay in my reply is that although I've managed to edit the dimensions associated with the mate, I'm still struggling to get the modified dimension to "stick" with the intended config. I spent a good half hour or more experimenting with it, trying to get closer to the desired outcome but still no cigar, just a butt-end for the moment. I can get 2 of 3 configs to work but the third insists on mimicking the first.

I'm suspecting that I may have got the default config caught up in the process when I should have simply added 3 derived configs perhaps. Certainly, I'm not fully there yet and this seems to be another one of those features that SW have struggled to implement intuitively. If / when I get there I will post what I found.

Murray

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Mike Helsinger @ Murray Edington on Nov 24, 2015 10:01 AM

Just in case you haven't caught these steps I'd like to add an illustration. Following Glenn's method you windows should look something like this

Also note this method of modifying dimensions by configuration applies to part features and sketches as well as assembly mates. If you have an extrusion you can modify it's depth in multiple configurations this way. You could also modify any / all dimensions in the configurations of a sketch.

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Craig Schultz Nov 24, 2015 8:09 AM

Murray,

Do you see the area highlighted in this pic when you try to edit the dimension?

It should give you the options of: this configuration, all configurations, specify configurations,......and link to parent (if it's a derived config). I'm guessing you might have one of them linked to parent. Just a guess though.

If you don't see these options, have you tried a design table which controls the dimension?

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Murray Edington @ Craig Schultz on Nov 24, 2015 9:18 AM

You see, this is where it all gets rather frustrating.

If I click on the highlighted (blue) dimension, then follow all the way through on "dimension", "options", "specify options", finally I get to the place I need to be.

You see, I would have thought that faced with this (below), by clicking on "properties" I'd get where I would need to be fairly rapidly. Guess I was wrong there. Silly me.

(Sorry, it lost the screenshot of the rollout you get when you right click on one of the configs but here is what you get):

Perhaps it's staring me in the face but that simply takes you (me) to a frustrating place with no answers. Is it me?

I guess the next thing is to actually check it out for real. I'll let you know what happens. If you don't hear from me, send in the troops....

Actions

Craig Schultz @ Murray Edington on Nov 24, 2015 9:30 AM

Just double click on the dimension. Then you should get the same input box that mine shows.

I think you're making it a little harder than it needs to be by going through those other menus.

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Glenn Schroeder Nov 24, 2015 9:43 AM

Murray,

Did you follow the instructions I gave above? Here are a couple of screenshots to explain. I right-clicked on the dimension in the graphics area. It's hard to see here, but it's circled. I then select "Configure Dimension" from the drop-down.

That brings up this dialog box.

This particular assembly only has one configuration, but if there were multiple configurations they would each have a row, and I could assign the desired value for each one in the appropriate box. I could also add new configurations here.

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Mark Kaiser Nov 24, 2015 10:13 AM

You are missing a basic SW concept of how to use configurations. Set up a simple assembly, and test it. If you can't get it, upload it and tell us what you want it to do. If your assembly you are having trouble with is not proprietary, upload it (and all it's parts, pack n go), and let us have a look.

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Murray Edington @ Mark Kaiser on Nov 25, 2015 7:59 AM

I've tried several times with just a nut and bolt. I've just created another one that actually worked, using the various hints above. Wahay! I'd been in this table before and failed to get it to behave.

If you look at the simple assembly I was struggling with yesterday, you may understand my frustration. I may have changed a hidden setting somewhere but the plan was to be able to set the nut 0mm, 6mm or 12mm from the end of the bolt. It will only go to 0mm or 10mm. 10mm was the original "alternative" distance.

If you can figure out why it's refusing to go to 6mm or 12mm, that might tell me where I have been going wrong! Any help gratefully received! Hopefully there is a simple explanation.

Murray

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Craig Schultz @ Murray Edington on Nov 25, 2015 8:14 AM

It works fine on my machine.....once I unsuppressed the distance mate in every configuration. I checked and every configuration had the right distance and "this configuration only" was selected.

If the mate is suppressed, it's going to leave the part in one position. Jody's way works as well if you want to suppress/unsuppress in every configuration = waste of time and added headaches.

Actions

Mark Kaiser @ Murray Edington on Nov 25, 2015 8:51 AM

I second Craig. It worked for me, but I had to unsupress the distance mate in a couple configs also.

One thing to help might be what faces you are mating to, and if the distance mate dimension is required to 'flip' between configurations (change its direction). This might cause issues.

With the mate being suppressed, maybe this is the only problem, and when you are adding new configs, it is auto suppressing for you. Here are some pics to check that.

Distance mate showing suppressed when I opened your assembly.

RMB on config, click on properties.

Actions

Murray Edington @ Mark Kaiser on Nov 30, 2015 7:39 AM

Thanks everyone. I had to select one of the many replies and label it the correct one. In practice there were several posts that told me where I was going wrong.

I've managed to set up several configs wit different positions and call them up in the drawings. I even managed to get 2 versions of a spring configured into the bargain.

Thanks for the help - much appreciated.

Murray

Actions

Jody Byram Nov 25, 2015 7:59 AM

Maybe its a brute force approach, but I was able to get it to work by creating multiple distance mates, and suppressing all but one of them in each configuration. SW complained as I was creating the redundant mates, but settled down once they were suppressed correctly.

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Tateos Tvapanyan @ Jody Byram on Nov 25, 2015 9:05 AM

I have done it at the same manner.

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14 Replies

Glenn Schroeder Nov 22, 2015 12:05 PM
Mark Correct
Correct Answer
Find the distance mate in the tree. Click on it (or double-click, depending on whether or not you have Dynamic Highlight turned on) to show the mate dimension in the graphics area. Right-click on it and choose "configure dimension" from the drop-down. That will open a simplified design table with a row for each configuration and a column for the mate dimension. Enter the desired value for each configuration in the appropriate cell. If you want, you can name and save the table near the bottom of the dialog box for future editing, but the changes will take effect even if you don't.
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- Murray Edington @ Glenn Schroeder on Nov 24, 2015 7:17 AM
  Mark Correct
  Correct Answer
  Thanks Glenn - that seems to be heading in the right direction, although I'm not out of the woods yet.
  
  The reason for the delay in my reply is that although I've managed to edit the dimensions associated with the mate, I'm still struggling to get the modified dimension to "stick" with the intended config. I spent a good half hour or more experimenting with it, trying to get closer to the desired outcome but still no cigar, just a butt-end for the moment. I can get 2 of 3 configs to work but the third insists on mimicking the first.
  
  I'm suspecting that I may have got the default config caught up in the process when I should have simply added 3 derived configs perhaps. Certainly, I'm not fully there yet and this seems to be another one of those features that SW have struggled to implement intuitively. If / when I get there I will post what I found.
  
  Murray
  Like • Show 0 Likes0
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  - Mike Helsinger @ Murray Edington on Nov 24, 2015 10:01 AM
    Mark Correct
    Correct Answer
    Just in case you haven't caught these steps I'd like to add an illustration. Following Glenn's method you windows should look something like this
    
    Also note this method of modifying dimensions by configuration applies to part features and sketches as well as assembly mates. If you have an extrusion you can modify it's depth in multiple configurations this way. You could also modify any / all dimensions in the configurations of a sketch.
    Like • Show 1 Like1
    Actions
Craig Schultz Nov 24, 2015 8:09 AM
Mark Correct
Correct Answer
Murray,

Do you see the area highlighted in this pic when you try to edit the dimension?

It should give you the options of: this configuration, all configurations, specify configurations,......and link to parent (if it's a derived config). I'm guessing you might have one of them linked to parent. Just a guess though.

If you don't see these options, have you tried a design table which controls the dimension?
Like • Show 1 Like1
Actions
- Murray Edington @ Craig Schultz on Nov 24, 2015 9:18 AM
  Mark Correct
  Correct Answer
  You see, this is where it all gets rather frustrating.
  
  If I click on the highlighted (blue) dimension, then follow all the way through on "dimension", "options", "specify options", finally I get to the place I need to be.
  You see, I would have thought that faced with this (below), by clicking on "properties" I'd get where I would need to be fairly rapidly. Guess I was wrong there. Silly me.
  
  (Sorry, it lost the screenshot of the rollout you get when you right click on one of the configs but here is what you get):
  
  Perhaps it's staring me in the face but that simply takes you (me) to a frustrating place with no answers. Is it me?
  
  I guess the next thing is to actually check it out for real. I'll let you know what happens. If you don't hear from me, send in the troops....
  Like • Show 0 Likes0
  Actions
  - Craig Schultz @ Murray Edington on Nov 24, 2015 9:30 AM
    Mark Correct
    Correct Answer
    Just double click on the dimension. Then you should get the same input box that mine shows.
    
    I think you're making it a little harder than it needs to be by going through those other menus.
    Like • Show 0 Likes0
    Actions
Glenn Schroeder Nov 24, 2015 9:43 AM
Mark Correct
Correct Answer
Murray,

Did you follow the instructions I gave above? Here are a couple of screenshots to explain. I right-clicked on the dimension in the graphics area. It's hard to see here, but it's circled. I then select "Configure Dimension" from the drop-down.

That brings up this dialog box.

This particular assembly only has one configuration, but if there were multiple configurations they would each have a row, and I could assign the desired value for each one in the appropriate box. I could also add new configurations here.
Like • Show 1 Like1
Actions
Mark Kaiser Nov 24, 2015 10:13 AM
Mark Correct
Correct Answer
You are missing a basic SW concept of how to use configurations. Set up a simple assembly, and test it. If you can't get it, upload it and tell us what you want it to do. If your assembly you are having trouble with is not proprietary, upload it (and all it's parts, pack n go), and let us have a look.
Like • Show 1 Like1
Actions
- Murray Edington @ Mark Kaiser on Nov 25, 2015 7:59 AM
  Mark Correct
  Correct Answer
  I've tried several times with just a nut and bolt. I've just created another one that actually worked, using the various hints above. Wahay! I'd been in this table before and failed to get it to behave.
  
  If you look at the simple assembly I was struggling with yesterday, you may understand my frustration. I may have changed a hidden setting somewhere but the plan was to be able to set the nut 0mm, 6mm or 12mm from the end of the bolt. It will only go to 0mm or 10mm. 10mm was the original "alternative" distance.
  
  If you can figure out why it's refusing to go to 6mm or 12mm, that might tell me where I have been going wrong! Any help gratefully received! Hopefully there is a simple explanation.
  
  Murray
  Attachments
  - Nut M12.SLDPRT.zip79.9 KB
  - Hex head M12x25.SLDPRT.zip109.1 KB
  - Config final.SLDASM.zip129.7 KB
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  - Craig Schultz @ Murray Edington on Nov 25, 2015 8:14 AM
    Mark Correct
    Correct Answer
    It works fine on my machine.....once I unsuppressed the distance mate in every configuration. I checked and every configuration had the right distance and "this configuration only" was selected.
    
    If the mate is suppressed, it's going to leave the part in one position. Jody's way works as well if you want to suppress/unsuppress in every configuration = waste of time and added headaches.
    Like • Show 1 Like1
    Actions
  - Mark Kaiser @ Murray Edington on Nov 25, 2015 8:51 AM
    Unmark Correct
    Correct Answer
    I second Craig. It worked for me, but I had to unsupress the distance mate in a couple configs also.
    
    One thing to help might be what faces you are mating to, and if the distance mate dimension is required to 'flip' between configurations (change its direction). This might cause issues.
    
    With the mate being suppressed, maybe this is the only problem, and when you are adding new configs, it is auto suppressing for you. Here are some pics to check that.
    
    Distance mate showing suppressed when I opened your assembly.
    
    RMB on config, click on properties.
    
    Make sure checkbox 'suppress new features and mates' is not checked. If you create the mate first, then add configs, this box will mess with you. Do not remember if it is a system/document option somewhere, this box for me is always unchecked.
    Like • Show 1 Like1
    Actions
    - Murray Edington @ Mark Kaiser on Nov 30, 2015 7:39 AM
      Mark Correct
      Correct Answer
      Thanks everyone. I had to select one of the many replies and label it the correct one. In practice there were several posts that told me where I was going wrong.
      
      I've managed to set up several configs wit different positions and call them up in the drawings. I even managed to get 2 versions of a spring configured into the bargain.
      
      Thanks for the help - much appreciated.
      
      Murray
      Like • Show 0 Likes0
      Actions
Jody Byram Nov 25, 2015 7:59 AM
Mark Correct
Correct Answer
Maybe its a brute force approach, but I was able to get it to work by creating multiple distance mates, and suppressing all but one of them in each configuration. SW complained as I was creating the redundant mates, but settled down once they were suppressed correctly.
Like • Show 2 Likes2
Actions
- Tateos Tvapanyan @ Jody Byram on Nov 25, 2015 9:05 AM
  Mark Correct
  Correct Answer
  I have done it at the same manner.
  Like • Show 0 Likes0
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Struggling with assembly configuration for controlling drawing views

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