Copy Design does not Copy fx used in iProperties field (2018)

[reverbbb]

 

I thought I had a simple idea of creating a corrugated box (5 panel folder) with sheet metal. That works great. The lid is hinged and needs to be shown open on a packaging drawing. Since this package is also used in a lager carton, I need to also show the carton as closed. I am a contractor working for a company that is still using 2018. 2018 does not have Design States. Therefore, I have not figured out a way to show the same box as open or closed within the same model. The only thing that changes is the angle of the lid (-45 degrees for open and 90 degrees for closed). I created a form for ease of use:

So, I decided this needs to be two models. I link the "BOX_WIDTH", "BOX_DEPTH", "BOX_HEIGHT" parameters of the Open box to the "BOX_WIDTH_CL", "BOX_DEPTH_CL", "BOX_HEIGHT_CL" parameters of the Closed box. My iLogic script is updating the Closed box when I open that model. I also use "= BOX <BOX_WIDTH> X <BOX_DEPTH> X <BOX_HEIGHT>" in the "iProperties"/"Description" field. All this is working great:

The Issue:

I want to use these two files as a templates for many sizes in the future. When I use Copy Design from Vault, The Description parameters turn into static text. This field will no longer update when I change the size of the box. If I copy to a new number from outside of the Vault, my iParameters stay intact, but my Linked parameters of the Closed box always point towards the linked parameters of the original Open box design, and not the new Open box part number (file name).

Is there some iLogic file copy script that will also update either the "iProperties"/"Description" parameter fields, OR update the Linked file name to the new file name?

I am also open for suggestions on how to get two versions from the same file name without have two different files to exchange information.

[AaronJoSmith]

I think I understand the issue, let me know if I don't. I would just add a "SetDescription" rule so that the part description is set with iLogic. This would be how your description is defined. I've had a similar issue and this is how I resolved it. Add a rule with this code:

iProperties.Value("Project", "Description") =  "Box " & BOX_WIDTH &" in X " & BOX_DEPTH & " in X "& BOX_HEIGHT &" in"

 Let me know if this solves the issue.

[reverbbb]

I think the concept will work for the Vault Copy Design scenario. That is what I prefer. However, I get error "Line 49 : End of statement expected." when I added this:

iProperties.Value("Project", "Description") = "BOX " & BOX_WIDTH " X " & BOX_DEPTH & " X " & BOX_HEIGHT

[WCrihfield]

Hi @reverbbb.  Maybe you can use an old trick I used to use for these types of scenarios (without Vault).  When I needed to see two different versions of the same model, such as open & closed versions, or bent and flat versions, I simply created the same model twice in the same model file (multi-body part file), then used two or more DVRs (DesignViewRepresentations).  In one DRV only the open version solid body(s) would be visible, while the closed version solid body would not be visible.  Then the opposite for another DVR.  Or you could use LODs (LevelOfDetailRepresentations) and suppress the feature that creates the 'other' version of the solid(s).  That way it is all in one model file.  Then when you create drawing views, you can set which DVR and/or LOD you want the view to represent.  This worked just fine most of the time.  It can be a little odd to deal with in super complex scenarios though.

[reverbbb]

@WCrihfield ,

I am not familiar with multi-body parts and have never used them. I didn't realize Inventor had this functionality.

The problem is, this box needs to be unfolded. So I used Sheet Metal to design everything. The blue highlighted surface in this image, was simple an added flange with an angle (that changes the box from open to closed). All the other sides are also flanges. I don't see any capability of adding another solid to this current design state. It seems that I would need to start over and use 3DModel/Extrude functions instead of  flanges.

I spent a lot of time debugging the added flanges to represent the way the box unfolds to a flat pattern. I am so close. My client is expecting me to move on to more product based tasks. I don't think they want me to spend much more time on redoing this model.

[WCrihfield]

So are you able to simply change the parameter value that represents the angle of that flange to change it from open to closed?  If so, you could create a copy of the final solid body that is in its open or closed position using the 'Copy Object' command on the Sheet Metal > Modify panel, then set that new surface body not translucent, and set its appearance the same as the regular part.  Then change the parameter controlling the angle of that flange to the other position.  The copied surface body will keep its original shape (parameter change will not effect it).  Then you will have two bodies that you can control the visibility of, one for each position.  Just a thought, and fairly quick to produce.

[reverbbb]

@WCrihfield 

That worked!

But is there a way to get this surface model to look like the Paper/Cardboard color?

[reverbbb · Accepted solution]

I guess it doesn't matter on a drawing, if the views are not shaded.

Thanks for the tips. Great lessons learned here.

[WCrihfield · Accepted solution]

Glad I was able to help.

You can right-click on the surface body that was created by the Copy Objects command, then uncheck the 'Translucent' if it is checked, then right-click that surface body again and choose Properties.  In that little dialog, you can choose an Appearance to apply to just that surface body.  The 'As Body' option may not be available, so you would have to manually select the same appearance from the list that the main part is using.  It's slightly annoying, but possible.  There is usually more than one way to do almost everything in Inventor.

[reverbbb]

Thanks again!

[reverbbb]

@WCrihfield :

I have been using a Form to change sizes of my carton and show the carton Open or Closed. All is working well. I now know that I need to re-establish a new Composite when I change the size of the carton. This is working as a manual set of commands.

However, I now want to share this master template file to co-workers. It is my desire that a background Marco runs and does the task of updating the CLOSED carton Composite. I am clueless on how to initiate that command sequence in an automated manor.

The idea is that a new user simply changes the carton size. Without any more interaction from the user, the "Sheet Metal>Modify>Copy Object>Select Existing" sequence is set in motion. The user would only need to pick the surface of the carton and the new CLOSED Composite would be generated. The final step would be to SaveAs a new Model/Part Number. This last step would need to be a user entry to establish the correct Part Number naming convention.

This is a screen shot of my Form:

The carton would need to be set in the "Closed" configuration before the automatic Copy Object is initiated:

Notice that I already have "Open" & "Closed" Views established. At this point, the user only needs to select the side of the carton. Then the SaveAs Dialog would pop-up.

If I can get this background automation to work, all of my coworkers would be able to create new carton sizes with very little instruction on how to do that task.