Solved: Re: Content Center Adaptivity

Anonymous · ‎03-08-2017

In Inventor 2017, I would like to use simple C-Channels from the content center, but I also need them to be adaptive in length in my assembly. Is this possible? When inserting from content center, it asks for a length that cannot be changed later on. I could either drive the length by constraints or by a Parameter, either would work for me in this case, but how??

Or do I have to actually draw the channel outline in a sketch and then extrude it and make it adaptive that way? Seems like the content center is somewhat useless if I have to draw these channels anyways...

I'm sure I'm missing something silly, please let me know if I am!

Thanks!!!

PaulMunford · ‎03-08-2017

Look into Frame Generator.

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johnsonshiue · ‎03-09-2017

Hi! I think you should be able to place a structure shape par as a custome partt from Content Center in an assembly. Next make the extrusion and the part adaptive. Then constrain the two adaptive workplanes in the part to other geometry in the assembly. It should work. Please note that the adaptive part is assembly specific. So, adaptive partA adapts within Assembly1 will not adapt in Assembly2. These custom CC parts will need to be separated on a per assembly basis.

Many thanks!

Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer

Anonymous · ‎03-09-2017

How do I place the content center part into the assembly without first having to give it a length? If I could place just the 2D sketch of the outline of the C-Channel, that would be great - then I could do as you suggest and extrude it adaptively.

Along the same concept here - in Solidworks, I could generate a layout sketch within an assembly and then create parts based upon that sketch. In Inventor, I tried laying out a 2D sketch in the Assembly, and then creating a new part with lengths based upon that sketch - but I cannot snap to anything in that sketch. WHY???????? Sometimes Inventor makes me want to bang my head against the wall. If it wasn't for the great way it handles creating bent sheetmetal parts off of a solid, I would probably go back and re-purchase SW.

I will also check out frame generator when I have another free moment - maybe that is the way to go.

Thanks for the help so far!

johnsonshiue · ‎03-09-2017

Hi! Have you tried the following workflow?

1) Go to Assemble tab -> Place from Content Center -> Structural Shapes -> pick a shape -> there will be a default length like 0.001; you can change it to anything -> make sure "As Custom" is checked -> Ok.

2) Edit the structural shape part in place -> right-click on the Extrusion feature -> check Adaptive. Return to top.

Now you can constrain the workplanes to other assembly geometry within the same assembly.

Please let me know if it works for you.

Many thanks!

Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer

jtylerbc · ‎03-09-2017

@Anonymous wrote:

How do I place the content center part into the assembly without first having to give it a length? If I could place just the 2D sketch of the outline of the C-Channel, that would be great - then I could do as you suggest and extrude it adaptively.

You don't. You give it a placeholder length, then follow @johnsonshiue's instructions. Be sure to actually constrain the work planes as he described, not the end faces of the channel. FYI, in your initial post you said that the length can't be changed after part creation. This is not the case. Edit your channel part, then go to Parameters. The length is controlled by parameter "B_L". This may seem like a convoluted way of editing the part, but the Content Center structural parts are really optimized to work with Frame Generator, rather than for manual editing.

nakedauto wrote:

Along the same concept here - in Solidworks, I could generate a layout sketch within an assembly and then create parts based upon that sketch. In Inventor, I tried laying out a 2D sketch in the Assembly, and then creating a new part with lengths based upon that sketch - but I cannot snap to anything in that sketch. WHY???????? Sometimes Inventor makes me want to bang my head against the wall. If it wasn't for the great way it handles creating bent sheetmetal parts off of a solid, I would probably go back and re-purchase SW.

They way you handle that in Inventor is to create a "Layout Part", and make your sketches in it. You get to the "Layout Part" by clicking the "Component" dropdown on the Assemble tab, then "Make Layout."

Aside from that, what you describe is essentially the way Frame Generator works, so I suspect you'd pick it up pretty easily.

As for why you can't snap to the assembly sketch instead, I have no answer other than "You just can't."

Anonymous · ‎03-09-2017

That was my first logical thought process as well. However, even though I select "as custom" when inserting the structural shape, I cannot access the "extrusion" to make it adaptive, when editing the new part in place. The only option I can see listed that makes sense is "driven length" - which sounds exactly like what I would need to change. However, when right-clicking on this, there is no option to make it "adaptive".

Also, I can physically go in and edit the "B_L" parameter while editing the part in place, however after going back to the assembly I cannot access the B_L parameter, even in the list of parameters. If I could access it, and set it to a value based on my equations, that would be acceptable as well, but I tried and cannot.

Simplified screenshot attached. The two longer rectangular tubes are for forklift pockets. I have a user-defined parameter that is the distance between these two tubes. The shorter tube needs to connect the longer two together, and needs to update when the user-defined parameter is changed. I could do this in the parameters list easily if I could access either the "driven length" or the "B_L" values but I cannot while editing the assembly. I would rather be able to make an adaptive part that could automatically update based on it's constraints - but again, I cannot make it "adaptive" - I have no option for it when inserting a content center file, as shown...

-Darren

johnsonshiue · ‎03-09-2017

Hi Darren,

You need to right-click on the Extrusion feature -> Adaptive, not on the Driven dimension. Let me know if it works.

Many thanks!

Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer

Anonymous · ‎03-09-2017

Ok, so the extrusion "feature" is just listed as "body" in the tree - I right-clicked on everything (so I thought) and couldn't find anything that listed "adaptive" as an option. However in the quick simple assembly I just created, when I right clicked on "body" - it was there! I made it adaptive and then went back to the model. I can constrain *either* the work planes OR the faces and it seems to work properly!

As suggested, I should constrain based on the work planes. Logically, I would "gut instinct" constrain by the faces. Why is constraining by the work planes a better option?

Thank you all SOOOOOOO much for the help so far - it's little things like this that really get me with Inventor. I know that there will be hurdles to overcome after using SW for 20 years, and that I'll have to re-train my way of doing things. But it's none the less frustrating, lol! In my mind currently - there is a specific feature of the inserted content center part actually named "driven length" - so why the heck (excuse my language please) would that not be the feature that you would "drive"???? It's just not logical to me. Why even put that there? Just call the "body" something like "extrusion" so that it is easily understood? I can see now that the little icon next to it is the icon for an extrusion and I should have caught that. But Inventor sure makes you work for it!!

In searching for a bit more help - with the inserted content center part, is there any way to drive the B_L parameter from the main assembly parameters list? For instance if I were to make a user parameter that is an equation, can that value be translated to a content center part value? I can see where that could come in very useful. I can certainly drive the parameters of user-created extruded parts, but it doesn't seem like the content center parts parameters are available.

Again, thank you all for the help. I will still check into the frame generator - that looks pretty neat! I didn't even realize it was there, lol.

jtylerbc · ‎03-09-2017

@Anonymous wrote:

Ok, so the extrusion "feature" is just listed as "body" in the tree - I right-clicked on everything (so I thought) and couldn't find anything that listed "adaptive" as an option. However in the quick simple assembly I just created, when I right clicked on "body" - it was there! I made it adaptive and then went back to the model. I can constrain *either* the work planes OR the faces and it seems to work properly!

As suggested, I should constrain based on the work planes. Logically, I would "gut instinct" constrain by the faces. Why is constraining by the work planes a better option?

Thank you all SOOOOOOO much for the help so far - it's little things like this that really get me with Inventor. I know that there will be hurdles to overcome after using SW for 20 years, and that I'll have to re-train my way of doing things. But it's none the less frustrating, lol! In my mind currently - there is a specific feature of the inserted content center part actually named "driven length" - so why the heck (excuse my language please) would that not be the feature that you would "drive"???? It's just not logical to me. Why even put that there? Just call the "body" something like "extrusion" so that it is easily understood? I can see now that the little icon next to it is the icon for an extrusion and I should have caught that. But Inventor sure makes you work for it!!

In searching for a bit more help - with the inserted content center part, is there any way to drive the B_L parameter from the main assembly parameters list? For instance if I were to make a user parameter that is an equation, can that value be translated to a content center part value? I can see where that could come in very useful. I can certainly drive the parameters of user-created extruded parts, but it doesn't seem like the content center parts parameters are available.

Again, thank you all for the help. I will still check into the frame generator - that looks pretty neat! I didn't even realize it was there, lol.

The Extrusion feature is defined as being between the Start and End planes, rather than being defined to extrude a certain distance. In my experience I had better luck using Adaptivity to move the planes, and then the Extrusion just follows along. When I did this in the past (it's been a while since I've needed to do this on something that wasn't already a Frame Generator project), there was some sort of trouble I had when I tried using the end faces. I don't remember exactly what it was (instability with updating, failing to update later on, just plain not working initially, etc.), but there was some sort of problem I ran into. If you got it to work, it may be fine - it's possible that what I experienced was a version-specific problem that no longer applies.

Like I mentioned before, the modeling for the CC structural parts is knowingly unusual. I don't think any user would ever intentionally build a part exactly that way. But that oddness has to do with the behind-the-scenes operation of Frame Generator. When you're using FG, you don't notice the strange setup, because it's operating in the background and you're controlling everything with your Layout part. The unfortunate side effect is that manual modeling with the CC structural shapes seems a little illogical.

Once placed, there is nothing inherently different about the CC part's parameters from any other part. Exactly what method are you referring to for "driving the parameters" from the assembly, that doesn't work on the CC parts?

Frame Generator is indeed a very powerful tool (with it's own quirks here and there, of course). I use it quite a bit, and highly recommend it.

Don't feel bad about the learning curve. It takes some time to get up to speed when you switch between any two systems. Most of us here would be just as lost if we were sitting down at SolidWorks - we'd probably be asking you for help instead.

Anonymous · ‎03-10-2017

@jtylerbc wrote:

The Extrusion feature is defined as being between the Start and End planes, rather than being defined to extrude a certain distance. In my experience I had better luck using Adaptivity to move the planes, and then the Extrusion just follows along. When I did this in the past (it's been a while since I've needed to do this on something that wasn't already a Frame Generator project), there was some sort of trouble I had when I tried using the end faces. I don't remember exactly what it was (instability with updating, failing to update later on, just plain not working initially, etc.), but there was some sort of problem I ran into. If you got it to work, it may be fine - it's possible that what I experienced was a version-specific problem that no longer applies.
Like I mentioned before, the modeling for the CC structural parts is knowingly unusual. I don't think any user would ever intentionally build a part exactly that way. But that oddness has to do with the behind-the-scenes operation of Frame Generator. When you're using FG, you don't notice the strange setup, because it's operating in the background and you're controlling everything with your Layout part. The unfortunate side effect is that manual modeling with the CC structural shapes seems a little illogical.
Once placed, there is nothing inherently different about the CC part's parameters from any other part. Exactly what method are you referring to for "driving the parameters" from the assembly, that doesn't work on the CC parts?
Frame Generator is indeed a very powerful tool (with it's own quirks here and there, of course). I use it quite a bit, and highly recommend it.
Don't feel bad about the learning curve. It takes some time to get up to speed when you switch between any two systems. Most of us here would be just as lost if we were sitting down at SolidWorks - we'd probably be asking you for help instead.

Good info, thanks once again 🙂

As far as "driving the parameters" issue goes... When I edit the CC part, I can access and change the "B_L" value at will. Much like I can (now, lol) make it adaptive in the main assembly if need be.

However, when I back out to the main assembly, and go to the parameters pop-up dialog box, the "B_L" value is non-existent. So if I were to say, create a user parameter of "fork_spacing" and then need the value of a CC part's B_L to be "fork_spacing / 2 + 10" or whatever equation I need, I cannot do this. I think all this is really a moot point though - negated by either using a "layout part sketch" or using the frame generator. I'm leaning towards using the frame generator, although I know nothing about it yet. I'm much more used to creating a layout in SW, but it seems like the Inventor Frame Generator is really specifically designed for doing exactly this type of thing, so I'll learn something new to hopefully be more productive in the future.

You have been a great resource here, thank you so much for the help!!

-Darren

jtylerbc · ‎03-10-2017

FG is most likely going to help you a lot.

Your issue with not being able to drive the parameter is a misunderstanding of what you're looking at in the Parameters dialog box. It shows the parameters of the active file, not the entire assembly structure. So when you're in a Part, you see all the part's parameters.

When you're in an Assembly, you see the Assembly's parameters (which consists mostly of constraint offsets). It doesn't drill down into the parts and show you their parameters, which is why you can't see B_L. There are tricks you can do using iLogic programming to get around that, but I don't know if you want to deal with that at this point.

PaulMunford · ‎03-11-2017

I don't know if this was mentioned, but the 'Driven Length' is the total length of the frame member. This is the value that you get back in the BOM.

The distance between the workplanes is the 'Driving' dimension, and is set by typing in a value, making it adaptive or using the member in a frame generator assembly.

This is useful becuase frame generator can also clean up your end treatments by applying mitres or profile cuts between members.

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2016...

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PaulMunford · ‎03-11-2017

Oh - and, if you open a frame generator part file directly, it has it's own browser.

If you click at the top of the browser, there is a filter which allows you to see the standard feature tree...

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Anonymous · ‎03-11-2017

Hey guys!

So I fooled around in Inventor last night for a while. I found the option for creating a layout - was just that I hadn't pulled down that menu yet. I got a simple 2D layout sketch made up very easily. I then added a frame, inserted some CC profiles along the lines of the layout sketch, and made myself my first "frame". It was very intuitive and simple to use. I even "re-used" some pieces in there, was able to easily get them into the correct orientation, and then fooled around with the mitering capabilities. I am impressed so far!! I have some designs to do in the near future where I can see this becoming a welcome addition to my CAD experience!

After creating the frame, I added some other CC parts, and was able to make them adaptive without issue. I constrained to some of the faces in the model, then made the "end plane" adaptive and constrained it to the model. After all that, I went back to the user parameters of the main assembly (that drive the layout sketch) and changed some values by a decent amount. Backed out, and the whole thing updated without any issues at all. Both the frame generated parts and the adaptive CC parts went about their business without a hitch. Way cool man!

I have come to a conclusion about one main difference between SW and INV: Inventor seems to require you to do things in a certain way - which can be the same as or different from SW - but it can be frustrating at times. However, the other side of that equation (I'm hoping my initial observation is correct at least) I think is that I'll have less times where I change something in a complicated model and have the whole thing just fall apart. That has happened so many times in SW to me (of course I'm also comparing apples to oranges here - my SW was many, many years out of date, and my Inventor is the latest, greatest version). I have trained myself in SW as to which way to put something together so that the chances of it falling apart are near zero any more, but that took a long learning curve. Although I have beat my head against the wall a couple times with INV so far, in all honesty it really hasn't been all that hard to learn. And there is definitely quite a bit of added functionality that will be a game-changer in my designs in the future.

Plus, there's this awesome community here that I found! I'm very appreciative to all the help I've received here already! Everyone seems to be not only willing to help, but understanding and kind about how they do it.

THANKS!!!!

Content Center Adaptivity

Content Center Adaptivity

Content Center Adaptivity

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