[eloid]

hello looking for a autodesk Inventor guru, have a igus e chain drawing downloaded from there web site.. try to figure out how to make motion with it as a assembly file... have some issues with it.

[tlharris]

I took a quick look at the Igus site... there are quite a lot of products listed there.
1) Which product are you working with?
2) Which version of Inventor? Are you trying to do a Dynamic Simulation, or just animate a component?

[eloid]

I took a quick look at the Igus site... there are quite a lot of products listed there.
1) Which product are you working with?
2) Which version of Inventor? Are you trying to do a Dynamic Simulation, or just animate a component?

hello
working with ver 8 inventor, I was try to model / animate the e chain in my assebly drawing....
I was using there classic e4/0 r77 series product

part number 77-10-100-0
http://www.igus.com/igus/wsearch2_i.asp

[Rube]

I'm pretty sure that you can not have dynamic movement within an assembly in an assembly. In other words the links would each have to be put in the final assembly individually.
That does seem a little silly though, maybe I just haven't found the setting.

[eloid]

I'm pretty sure that you can not have dynamic movement within an assembly in an assembly. In other words the links would each have to be put in the final assembly individually.
That does seem a little silly though, maybe I just haven't found the setting.

so to understand you, because im new to inventor, you basically have to
place one link in your assembly drawing add addtional links as needed
build the chain etc ....then ground the one end etc.. for movement?

I think im have problems with the file as you described.... i think there a option to down indivuals parts ....have to explore it more...

[Rube]

so to understand you, because im new to inventor, you basically have to
place one link in your assembly drawing add addtional links as needed
build the chain etc ....then ground the one end etc.. for movement?

I think im have problems with the file as you described.... i think there a option to down indivuals parts ....have to explore it more...

Yes that is correct (it is how I have always done movable assemblies in other larger assemblies). If you open the chain assembly on its own, can you make it move like you are expecting? If they didn't have movable constraints on it in the first place, no matter what you do it won't move in your assembly.

Also, be careful when you say "...ground the one end...". Because if that fixed end of the chain is on another movable part, like a router gantry, and you "ground" the link, you will not be able to move the gantry. Your assembly probably already has some other part, like a base or table, already grounded, so the chian end should only be contrained to the component it is mounted too, but NOT neccessarily grounded. Does that make sense?

HMMMM...writing that I just thought of something. I'm going to do some experiments and if I find other than what I posted, I'll let you know.

[tlharris]

To be perfectly honest, I switched to Inventor at release 2008 - I don't know very much about the capabilities of v8.

Unfortunately, I use 2010 Pro, and there's no good way to save backward-compatible files, but here's how I'd do it:

1) I find the best success with STP files, which give you the whole assembly. Throw away what you don't need.
2) In this case, you only need 2 parts - one 'outer' plate, and one 'joining' plate. Create an individual link assembly using 2 of each of these. (4 occurences total)
3) Create an echain assembly, with the appropriate number of link assemblies. Ground the first one. Each additional link is constrained axially to the last one, and then face-to-face to keep them in line.
4) Insert the echain assembly into your router assembly. Make sure it's tagged FLEXIBLE (or it won't articulate the way you need it to)
5) Constrain the echain fixed end as required.
6) Constrain the echain movable (gantry) end to the gantry as required.

Your assembly should now move properly.

[Rube]

...Make sure it's tagged FLEXIBLE (or it won't articulate the way you need it to)...

Well...that's what I was missing. I knew there had to be a way to do it, but honestly didn't look hard enough. goes to show ya, you can ALWAYS learn something. I've been using Inventor since version ONE! Just self taught though.

[tlharris]

Right on..... glad it worked!

[eloid]

To be perfectly honest, I switched to Inventor at release 2008 - I don't know very much about the capabilities of v8.

Unfortunately, I use 2010 Pro, and there's no good way to save backward-compatible files, but here's how I'd do it:

1) I find the best success with STP files, which give you the whole assembly. Throw away what you don't need.
2) In this case, you only need 2 parts - one 'outer' plate, and one 'joining' plate. Create an individual link assembly using 2 of each of these. (4 occurences total)
3) Create an echain assembly, with the appropriate number of link assemblies. Ground the first one. Each additional link is constrained axially to the last one, and then face-to-face to keep them in line.
4) Insert the echain assembly into your router assembly. Make sure it's tagged FLEXIBLE (or it won't articulate the way you need it to)
5) Constrain the echain fixed end as required.
6) Constrain the echain movable (gantry) end to the gantry as required.

Your assembly should now move properly.

Im going to have to try this,,, over the holidays... soooooo..
if i have questions ..i will post them....

thanks for now.. i like i said im new to the enviroment so i have play with
it to fully understand it.

I also herd that you can get fre version of inventor 10, if your a stundent... is it any different then the pro version?

[eloid]

attached is a single link of the igus link... the question i have, the drawing is
a general shape ...doesnt include a stop face, is the way to make a constrate
without a face or edge ie tell it to bend to this angle ...the model from the web site does have the full detail of the stop blocks...

so there are issues constraining the bend? without modifing the model?
compete part number which is 77-10-100-0
http://igus.kimweb.de/index.asp?la=e...nr=77.10.100.0

is there way to wing it?

[eloid]

tlharris / Rube

i was hoping you can comment on my newest problem?

[Rube]

attached is a single link of the igus link... the question i have, the drawing is
a general shape ...doesnt include a stop face, is the way to make a constrate
without a face or edge ie tell it to bend to this angle ...the model from the web site does have the full detail of the stop blocks...

so there are issues constraining the bend? without modifing the model?
compete part number which is 77-10-100-0
http://igus.kimweb.de/index.asp?la=e...nr=77.10.100.0

is there way to wing it?

Your attached file is an assembly, but you didn't include the individual part files. I'll assume you just opened the assembly and deleted all the extra links and resaved it. Inventor still thinks it is an assembly with one part, and is looking for that part file.

No matter though. Angles are not the way to do this chain. You would need to do two constraints to each link. one would be a face to face mate to constrain the ears of one inside the ears of the previous one. Then a centerline to centerline mate on the rounded edges of the ears. This is how TL described it above. This would allow the articulation as expected.

I am using 2010 PRO so I cant create an assembly for you because you would not be able to open it.

[tlharris]

Sorry for the delay... but Rube's already covered it.

FWIW, the reason I asked about the Dynamic Simulation thing was that, although Inventor can indeed handle the actual constraints, the math involved is pretty complex when you start dragging this thing around. Dynamic Sim is a more advanced simulation available in Inventor Pro, where you could actually throw in some spring forces and gravity to provide more realistic movement. Without Dynamic Sim, some of the links can move a little strangely (mathematically correct, but may not be what you expect) Dynamic Sim is very possible, but it's a bunch of work if all you're attempting to do is make a picture. IV Pro (or Routed Systems) will also allow you to model each wire in the chase, but again, it can be a bunch of work.

Just a thought.

[eloid]

Your attached file is an assembly, but you didn't include the individual part files. I'll assume you just opened the assembly and deleted all the extra links and resaved it. Inventor still thinks it is an assembly with one part, and is looking for that part file.
hmmm

The way the side pcs are made, they dont have any built in stops? to prevent the raduis from being to large or small
the chain i have has ~10 dia.... i kinda understand how you suggest the contraint /But would the chain still pivoit beyoond the stop point due to no stop face constraint on the pivot point...


No matter though. Angles are not the way to do this chain. You would need to do two constraints to each link. one would be a face to face mate to constrain the ears of one inside the ears of the previous one. Then a centerline to centerline mate on the rounded edges of the ears. This is how TL described it above. This would allow the articulation as expected.

I am using 2010 PRO so I cant create an assembly for you because you would not be able to open it.

[Rube]

Yeah, it would be allowed rotate past what you would expect in the normal operation of the chain. The problem with adding an angle constraint to the links as well, is that when you try to drag the chain, it wont move because the angle is fixed. Again, you are testing my knowledge. I don't know of a way to give it a range of angles to move within. Now that I think of it too, even if we were able to do that, you would be able to pull the chain, but would not be able to push it back. kind of like a wet noodle. Once I think of the solution, I will be smaking my forhead. Maybe I'll download the link and give it a go.

[eloid]

ok im retring this idea...(I need it now for cnc model) a echain drawn in inventor 2010... made all the parts etc for the chain.... created a new the assembly for one "link" included contraints etc saved it.

created new assembly add above 3 "links"

I mated the links with each other along the rotation axis ..... nopblem...
this my problem....how can limit the rotation againt the stops on each link?
such that it will emulate a real chain with build in stops

see drawing

please explain or tell where to view a tutorial on this im lost?

[ger21]

When I did one in SW I used collision detection. For a larger chain, angle constraints would put much less load on the PC.

[eloid]

When I did one in SW I used collision detection. For a larger chain, angle constraints would put much less load on the PC.

i have to see if inventor has collision detection and how to use it?

[lostmyed]

I don’t believe it is possible (without Dy-Sim); I have tried numerous times and never got it to work. Inventor struggles after about 3 or 4 links are put together because it doesn’t know where within that angle range it needs to be. I have found the better way is to create the chain as a single part and drive it from an adaptive sketch from within your assembly. (it isnt going to look as good but it does work, and its easy)

Let me know if you struggle and I will see if a can dig out a part and give a better explanation.