Derived & mirrored sheet metal parts - application settings question

[llorden4]

In searching the forums, I see that it's been discussed here that mirrored sheet metal parts are not unfolding until you open the created mirrored part drawing and adjusting the sheet metal rules to the original styles the originating part was drawn from.  Is there an application setting I need to adjust in order to get these rules copied into the automatically generated mirrored file or is this just a feature lacking in the software.  If it's a lacking feature, who's the appropriate person we need to nag to get this feature added to the automation set?

Also on this subject is the file updating of the mirrored part.  I just learned the hard way that if you edit your parts from the assembly file, your derived mirrored parts update nicely but when it comes time to save your work the mirrored parts that have been updated do not automatically flag as "YES" for save like the originating part does.  You have to manually search through the list of components to find the mirrored part and select YES for the save.  True you could select YES to all but there are times you do not want to update all files.  Is there an application setting I need to alter that handles this aspect of flagging for save or is this just a feature oversight?  If an oversight, who's the appropriate person to nag for it's addition to the automation process?

If you're interesting in knowning how to get your derived mirrored part back without deleting and re-mirroring the part, what I did was to edit the original part, update the assembly (mirrored part now updates to match), and then edit the originating part again back to my desired values and update the assembly.  Now with the mirrored part updated correctly, save the drawing and be sure to flag the mirrored part file as "YES" for save.

[innovatenate]

In order to retain the sheet metal rule in the derived part, try setting up a sheet metal template containing the preferred defaults and settings. To do this, open a new sheet metal part and configure the desired settings, including Color, Sheet Metal Rule default, Sheet Metal Unfold Rule, etc... Don't forget to update your Styles and Standards! Next, perform a Save Copy as Template to make the template available in the New file dialogue box. You should be able to use this new template in both the original and the derived part to insure that the correct bend/rules settings are on by default. I've uploaded a word document with a few screenshots and some files for clarification. In the Save tab of Application Options, checking the "Prompt to save for re-computable updates" should automatically change the prompt to "Yes" for the mirrored or derived parts.

[llorden4]

I understand what your are suggesting is to create a new template and then edit the "DEFAULT" sheet metal rules with my desired settings so that any mirrored parts will use these desired (now "DEFAULT") values to save me the trouble of opening the automatically created mirror file and manually editing the sheet metal rules to the desired rule/setting I require.

If I only used one type of sheet metal ever, then this would be a solution.  Perhaps you mean to have a different template for each material type and not use the capability of having multiple rules assigned within one template.  The issue at hand is that I have to use different types of materials and I have several rules created for each type.  The mirrored file created copies of those rules into the file from the original part, what is not happening is the file is not saving the active rule used to create the originating part.  So if part "A" is created using a rule name "14 GA SHEET METAL" and I mirror that part to create part "A-MIR", the active rule of part "A-MIR" is "DEFAULT" and not "14 GA SHEET METAL" even though the rule is available from within the drawing.

So the question is does Inventor 2012 have the capability via some setting to keep the same Sheet Metal Rule active in the mirrored part file that its creating part is derived from other than limiting myself to only one type of material?  If not, I would ask that this be passed to the development teams to have this feature added for a future release.  In the meantime, I think I'd rather open and edit the rule of the created part rather than create a slurry of new template files to track and maintain.

Thank you for pointing out the solution to my other question forcing a "YES" flag for the re-computable updates.

[innovatenate]

For clarity, I was suggesting creating templates based on the actual sheet metal that you expect to form the parts from. The New File dialogue box image below is an example of what I mean.

 

There is a previously documented scenario that can prevent derived sheet metal parts from generating flat patterns or unfolding. When derived/mirrored sheet metal do not have matching thicknesses/Sheet Metal & Unfold Rules to the parent sheet metal file, the creation of flat patterns or unfolds may fail. To avoid this and to gain some uniformity in bend radii (since the default bend radii can be set in each template), I recommend the use of templates to simplify the creation of mirrored sheet metal parts.

[llorden4]

I understand what you're saying, I do.  What you're explaining is a type of work around and I already have a work around so that is not my question.  But let's keep going with your suggestion here for a moment in hopes you can understand where I'm coming from.

Let's create a new sheet metal part using one of the created templates as you have been suggesting, say using 16ga sheet metal.  I could create this part using the template at the .IPT level but I couldn't from within an .IAM file if I wanted to do a "top down" design (which is how I'd prefer to design).  So we create our first part, close the file and start a new assembly .IAM file and place our first part within the file.  Your option now stops me from being able to use the option of creating a new part (derived) from within the assembly file.  If I knew exactly what dimensions and features I wanted, then sure I can start a new part file and create a new file using the desired template and insert it into the assembly, but then the part is not a derived part.  If I were to setup template .IAM files with rules for each type of sheet metal, then I'd be limited to one type of sheet metal for use in the entire project with the goal in mind of not having to edit the sheet metal rules of the generated part files.

Am I correct on this process or is there another approach I'm not aware of?  From what I understand of Inventor, the Sheet Metal Rules, and not the template, is the driving force behind derived sheet metal components.

[innovatenate]

I apologize for the clarity of my earlier message. I understand now you are searching for an enhancement that would allow sheet metal files created from the Mirror feature, located on the Assemble Ribbon in the Component section, to assume uniform properties of the parent part from which it was generated. Otherwise, the mirrored component will assume the default sheet metal rules

. 

If this is correct, I will make a submission to development on your behalf. Just let me know.

To continue the work-around discussion, using the Derive feature from the Manage Ribbon in the Insert Section may take a similar amount of time. This workflow will allow you to utilize templates to bypass modifying sheet metal rules. Attached is a file showing how the Derive workflow can be used in a Top-down approach. Please review the attachment and let me know if it helps.

While this workflow may be less than ideal, the mirror component and derive feature serves a broader scope than just sheet metal parts. The ability to maintain rules between sheet metal components would be an enhancement to the current functionality.

Thanks,

[llorden4]

Yes, that's it exactly.  If there isn't a setting already that I can toggle that will allow the mirrored components to keep the properties (and update should the parent properties change) then I indeed I would like the developers to consider adding this capability.  Like you've pointed out, there are work arounds but with all the automation to get this far, it makes sense to go that extra half an inch and match properties during the creation process.  I hope others agree.

[SBix26]

I don't do much with sheet metal, so I haven't run into this issue, but I agree that this would be a smart and logical enhancement to Inventor.

[gavbath]

I agree that this is a much needed fix to the currently "not quite finished" functionality. I can only assume that this was an oversight. If a mirrored component is a true mirror, then all the geometry should be the same dimensions but opposite hand (unless reused.) If a 3mm thick sheetmetal part is mirrored and then the original part has it's thickness changed to 4mm thick, then the mirrored part should also change to be consistent with the way the mirror tool works for all other geometry changes.

Please fix this ASAP.

[BLHDrafting]

I also agree. While creating a myriad of templates may work it is unpractical in a real world setting. This should be added to the Wishlist here :-

http://www.augi.com/wishlist

[gavbath]

I've realised that my previous post is actually not quite correct. Because the mirrored sheetmetal part is actually derived from the original sheetmetal part, it will actually use the original part's thickness to control it's geometry, not the sheetmetal style. Changing the style in the original part (and therefore the thickness) will also change the mirrored component. I still believe however, that the style of the mirrored part should match the original automatically to allow unfolding.