Frame Generator Double Trim Cut Length

[gcoombridge]

Hi All,

First off I'm using Inventor 2017.4.1

This issue has played out a number of times in the forum but I'm going to raise it again because it has wasted hours of my day. I feel like I understand the issue quite well so I'm more pleading with Autodesk to fix it than anything...

Frame generator assemblies where either one or both ends of a member have 2 trim to face end treatments only regard the first end treatment when calculating the base quantity cut length. I.e. the first cut you make (on each end) sets the G_L parameter that reads out on the drawing page no matter what the actual length of the finished member is.

In principle I don't have a problem with this because it makes sense in a way. You put a length of steel in a bandsaw and make the first cuts, and then the second set - you can't zig-zag your cuts to suit (unless you laser cut). Where this falls apart is it totally depends on which end treatment you make first as to what you final cut length read out is.

I'm in a situation where I'm making large and fairly complex platforms that are the mirror image of each other. 

My workflow is that I make a skeleton sketch for the first one and derive with a mirror operation for the second. Because of this end treatment issue my cut lists for what are essentially identical frames come out different unless I meticulously follow the same order of trim features! It's always fixable but is really time-consuming and as a result I don't trust the results without fully auditing them by printing two lists side-by-side with a marker pen in hand.

I know the beinginventive guys posted this years ago (http://beinginventive.typepad.com/being-inventive/2011/06/double-mitered-frames-report-the-wrong-fra...) but it sounds like it needs a lot of updating and doesn't work with curves.

I've attached a couple of images to demonstrate the issue... I trimmed using the red members as the cutting plane first.

Thanks

Glenn

[jmenier]

What happens if you trim using the blue parts first on the left assembly, then red on the right assembly... could it be order of operations that are getting you?

no idea if this would work, just wondering.

[johnsonshiue]

Hi! This is a limitation right now. We are aware of it and we are investigating a good solution to it.

Many thanks!

[jtylerbc]

@johnsonshiue,

I believe I've mentioned this in threads here before, but we had previously experienced this sort of issue (maybe not this exact scenario, but the general idea of the reported lengths being incorrect) in the past.  A few years ago, I resolved it on our end with an iLogic rule that simply measures the extents of the part in the length direction (Z).

Using this method, the resulting length reported is always the same, regardless of how the tube was modeled.  This is particularly important in our case because while we do often use Frame Generator, we also use the CC structural parts as components in weldments that are not created using FG.  This method gives consistent results either way.

If they aren't already, Autodesk might want to consider doing something similar that is based on automatically measuring the final resulting model, rather than trying to keep up with the length by adjusting parameters.  I've found it to be much more reliable.  Since introducing the rule 3-4 years ago, I have not heard of a single case where a structural part's length was incorrect in a Part's List.

[gcoombridge]

Hi @jmenier

That's exactly what the issue is... The order of operations is easy to manage to the simple example I provided for illustration but when you have large assemblies and multiple frames that have LH and RH orientations it becomes VERY hard to manage. It would be much simpler if Inventor just read the finished length.

Thanks

[gcoombridge]

Hi @jtylerbc,

Thanks, I think this may be my answer too. The downside is that I was keen to start doing guard railing as frame generator assemblies to provide accurate cut lists and these typically involve curved sections. If you generate the cut length from the bounding box or the z extrusion length on a curved part you surely won't get a correct result?

Hi @johnsonshiue thanks for your reply - I hope you guys can come up with something soon... This is a problem that has persisted for the 11 years I've been using inventor! It may be unfair but I feel like the core of the product improves in leaps and bounds while the peripheral tools like frame generator and tube and pipe don't get the attention that they should...

Thanks

[jtylerbc]

---

@gcoombridge wrote:

Hi @jtylerbc,

Thanks, I think this may be my answer too. The downside is that I was keen to start doing guard railing as frame generator assemblies to provide accurate cut lists and these typically involve curved sections. If you generate the cut length from the bounding box or the z extrusion length on a curved part you surely won't get a correct result?

---

For curved sections, my method would definitely not work.  It just measures the part extents in the Z direction (all CC structural shapes are extruded in this same direction).  It was never intended to work on curved members.  We don't typically use them, so it wasn't really a consideration for me when I developed my solution.

[Mark.Valenti]

I am new to iLogic, and not very good at programming. can you post the code that allowed you to do this?

[Mark.Valenti]

I am new to iLogic, and not very good at programming. can you post the code that allowed you to do this?

---

@jtylerbc wrote:

@johnsonshiue,

I believe I've mentioned this in threads here before, but we had previously experienced this sort of issue (maybe not this exact scenario, but the general idea of the reported lengths being incorrect) in the past.  A few years ago, I resolved it on our end with an iLogic rule that simply measures the extents of the part in the length direction (Z).

Using this method, the resulting length reported is always the same, regardless of how the tube was modeled.  This is particularly important in our case because while we do often use Frame Generator, we also use the CC structural parts as components in weldments that are not created using FG.  This method gives consistent results either way.

If they aren't already, Autodesk might want to consider doing something similar that is based on automatically measuring the final resulting model, rather than trying to keep up with the length by adjusting parameters.  I've found it to be much more reliable.  Since introducing the rule 3-4 years ago, I have not heard of a single case where a structural part's length was incorrect in a Part's List.

---

[jtylerbc]

@Mark.Valenti, I think I have posted it on these forums before, but am not sure where, so here it is again.  Comments in the code explain a bit about what is being done.  It's actually a pretty simple piece of code, which has saved a ton of time at my company.

The code as-is writes the measured value to a User Parameter called "LENGTH_DESC".  This parameter is then embedded in the part's Description in our case, but alternatively be a Parts List column of its own.  The parameter can be renamed as needed to fit your situation.  We set Event Triggers for this rule as "Before Save" and "Part Geometry Change". 

' This rule uses the Measured Extents in the Z direction to develop a parameter which will be used in the material list description.

On Error Resume Next

oDoc = ThisDoc.Document
' Verify that the document is fully updated prior to taking measurements.
InventorVb.DocumentUpdate()
' Work features will be included in the extents if they are visible, which interferes with accurate measurement.
' Object visibility of work features and surfaces will be set to invisible before the measurements are taken, then returned to their previous state.


'toggle construction surface visibility off
oDoc.ObjectVisibility.AllWorkFeatures = False
oDoc.ObjectVisibility.ConstructionSurfaces = False
oDoc.ObjectVisibility.Sketches = False
oDoc.ObjectVisibility.Sketches3D = False

' Determine the extents of the part in Z direction
' Assign the measured value to the LENGTH_DESC user parameter
LENGTH_DESC = Measure.ExtentsHeight

'toggle construction surface visibility on
oDoc.ObjectVisibility.AllWorkFeatures = True
oDoc.ObjectVisibility.ConstructionSurfaces = True
oDoc.ObjectVisibility.Sketches = True
oDoc.ObjectVisibility.Sketches3D = True

' Update so changes are visible to the user
RuleParametersOutput()
InventorVb.DocumentUpdate()

[Mark.Valenti]

Awesome! thank you!!

[Anonymous]

Is this meant to pull the length of one side of a frame member with a double end treatment? I need the length to be pulled from only one face of a double miter (see picture). I have been unsuccessfully trying to get this dimension to come up accurately in my parts/cutlist for a few days now. I've tried the iLogic code that you provided and it didn't work. I also tried the one for double mitered frame members from several years ago but it doesn't seem to be working on Inventor 2019. Thank you for your time.

Marvin 

[jtylerbc]

@Anonymous,

If I'm understanding your question correctly, no.  My code gives the overall length.  So on a part that is mitered on both ends, the dimension it gives would be from the point on one end to the point on the other end. 

If the overall extent is what you are looking for, it works very well, and will give the correct value no matter what end treatments or other features are used to produce the part.  If you're looking for any other dimension, then it's not going to be of any help. 

[Anonymous]

Yes you're understanding correctly. I don't want the overall length from point to point so I guess yours won't work. Do you know if there's a way to accurately get the length from the point on one side to the short end on the other? When I create a cutlist, I give the fabricators the angle and the dimension from long side to short side. Your code would definitely work if the miters are opposite directions \ / but not if they're the same direction //. Thank you for your response; if you know of a way to accomplish what I need I appreciate it. Thank you for your time.

Marvin 

[jtylerbc]

@Anonymous, since you already have your own thread for your issue, I posted the only suggestion I can think of for your specific situation there.

This thread was originally referring to a different problem, where frame members mitered twice on the same end reported an incorrect overall length (using the built-in G_L parameter).  My iLogic rule solution can resolve that problem, since it ignores the built-in parameters entirely and just measures the length of the final part, regardless of how the part was created.

It does not resolve your situation , and I don't really see a way it could be adapted to do so.

[lena.talkhina]

Hello @gcoombridge  !

Great to see you here on Inventor Forum.

Did you find a solution?
If yes, please click on the "Accept as Solution" button as then also other community users can easily find and benefit from the information.
If not please don't hesitate to give an update here in your topic so all members know what ́s the progression on your question is and what might be helpful to achieve what you ́re looking for. 🙂

[gcoombridge]

Hi Lena, 

The solution was that Autodesk finally fixed the problem in 2019 I think.. Good discussion here though

[lena.talkhina]

Hi @gcoombridge !

Thank you for coming back to this thread and letting us know that the issue was solved with the update.
Me and the whole community team appreciate your impact.