Community
Inventor Forum
Welcome to Autodesk’s Inventor Forums. Share your knowledge, ask questions, and explore popular Inventor topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

assembly constraints and other Qs

37 REPLIES 37
Reply
Message 1 of 38
oneloosecrank
1358 Views, 37 Replies

assembly constraints and other Qs

Hi all, 

First off - my questions are of the fairly basic variety and I seem to be amongst rather more complex queries. Is this the best place for me or is there a 'beginners' area?

Questions then; I'm assembling a number of components and my first project is coming along quite well. It is a fulll suspension bicycle frame. The rear wheel is suspended from the frame by two pairs of linkages. Now, I've got my constraints sorted (axis and faces) to have the links located where I want them but when I move the linkages, they push the frame around as well rather than simply spin on the axis. The links are also constrained to move in tandem by way of constrained axis. How can I make the frame a 'fixed' entity with everything moving around it, or the constraint?

Next, I've got a lot of unwanted things in my workspace that I'm struggling to hide / remove. Dimensions on the link (I've tried going into the sketch but they won't delete from there), a worklplane I don't really want to be looking at and yellow lines which I think are the from a 'sweep' extrude. How do I go about cleaning up the assembly?

Finally, if you look at the attached project, you'll see that I need a rear triangle which will be the hardest thing I've started on because of it's depth (both sides will be of a single structure so I can't design one side then mirror it). Could you give me a hand with the best direction to approach this from?

With thanks

37 REPLIES 37
Message 2 of 38
blair
in reply to: oneloosecrank

You need to have at least one component "Grounded". In this case the frame might be the best choice. Simply RMB on the frame either in the assembly window of browser window and select "Ground Component".

 

The sketch looks like it's a uncomsumed sketch in the component. You should be able to open the part and delete the sketch in the browser window.

 

You can either RMB on the work plane and toggle it's visibility on/off or on a global scale for the assembly from the View>Visibility>User Work Planes.

 

If you give some thought as to how the triangular link is going to be made in real life it would give you some insight into how to model it in IV.

 

If it is going to be machined from a solid block of aluminum, you could simply extrude a primary shape the overall thickness of this part and then "machine" (sketch-extrude-cut) sections out of the block to get your part.

 

You could create one side/half of the part and mirror the other side.

 

If it is made up of smaller parts, create a sub-assembly with one side part, derive/mirror the part for the other side if they are LH and RH with a couple of connecting parts.


Inventor 2020, In-Cad, Simulation Mechanical

Just insert the picture rather than attaching it as a file
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.
Delta Tau Chi ΔΤΧ

Message 3 of 38
JDMather
in reply to: oneloosecrank


@oneloosecrank wrote:
... Could you give me a hand with the best direction to approach this from?

With thanks


Attach your assembly here.


-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


EESignature

Message 4 of 38
oneloosecrank
in reply to: JDMather

Assembly attached. The 'grounded' aspect looks to be thing I need. However Inventor is having an issue and wants to redefine a plane? Not sure what this means.

Message 5 of 38
JDMather
in reply to: oneloosecrank

An assembly file (*.iam) is only a list of hyperlinks to the part files (*.ipt) and a record of assembly constraints (and a bit more).

You must include the part files.


-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


EESignature

Message 6 of 38

 
Message 7 of 38

 
Message 8 of 38

That's all the part files and the assembly.

Message 9 of 38
oneloosecrank
in reply to: blair


@Blair wrote:

 

If you give some thought as to how the triangular link is going to be made in real life it would give you some insight into how to model it in IV.

 

If it is going to be machined from a solid block of aluminum, you could simply extrude a primary shape the overall thickness of this part and then "machine" (sketch-extrude-cut) sections out of the block to get your part.

 

You could create one side/half of the part and mirror the other side.

 

If it is made up of smaller parts, create a sub-assembly with one side part, derive/mirror the part for the other side if they are LH and RH with a couple of connecting parts.


Well, it would be made up of three machined parts and four beams all welded together. I started out this morning with a large box which would encompass the whole rear end of the frame and started cutting in to it but I don't think I can go much further. It's not going to be the right approach as various parts aren't symetrical. So... I'll have to take your advice on creating a sub assembly and make each machined part individually. I should be able to make one side and then mirror it. 

Message 10 of 38
JDMather
in reply to: oneloosecrank

Before I spend a lot of time on this - how dedicated/serious are you about finishing the project?

Is it a school assignment that is due Friday?

 

The reason I ask, is it seems as soon as I spend a couple of hours helping someone they disappear.

 


-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


EESignature

Message 11 of 38

I completely understand. As a regular contributor in another community, it's a real bore when we take time to assist someone who then dissapears never to be heard from again. My aim is to fabricate this very design as a prototype to a future bike. I have spent the last year coming up with a design that I have intend to build and maybe in the future sell. However, whilst I can design frames on paper, I do need to learn cad to get dimensions and part files for cncing.
Message 12 of 38

I intend to be around cad for a while and will probably be asking lots of questions until I can produce independently. Sorry for double post, phone wouldn't let me edit the first.
Message 13 of 38
JDMather
in reply to: oneloosecrank

If you are persistant the users here will help you for as long as it takes.

 

You did not include the part Main triangle.ipt in this thread.

I have an earlier part with that name, but Inventor does not see it as your current assembly part and I get constraint errors. 

 

Can you attach your current Main triangle.ipt here.

 

I notice that most of your part sketches are not fully defined.

I recommend reading this

http://home.pct.edu/~jmather/SkillsUSA%20University.pdf

 

 


-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


EESignature

Message 14 of 38

Ah OK, will do. I'll attach when I go in for lunch. I think this define sketches is causing me lots of issues - I'll need to study up on that. Cheers
Message 15 of 38

Triangle attached. The yoke might be needed as well now as I started on it this morning.

Message 16 of 38
JDMather
in reply to: oneloosecrank

Once you learn how Inventor assigns assembly constraints - most of the work is done by Inventor for you automatically.

For example, by click, hold and drag a line off of an arc - the Tangent Constraint is added automatically.  By click, hold and drag off of a line endpoint (while still in the line command) an tangent arc can be created.

 

Zoom (way) in on the location in attached image.

What do you see?

 

Why you are fixing this - add tangents to your arcs and lines.

 

In order for me to manufacture something out on the shop floor - it should be fully defined.

So why shouldn't the designer do this work before sending to manufacturing?

 

 


-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


EESignature

Message 17 of 38
JDMather
in reply to: JDMather

At your level of experience you should probably NOT be creating sketches at the assembly level.  (see attached image)

And probably not axis or workplanes.

 

If you want to define the locations of the tires/wheels relative to the frame, then create a sketch in the Main traingle.ipt file that you can then use in the assembly to constrain the tyre and rim.ipt.

 

I recommend that you start investigating multi-body solids (master modeling) techniques were you model all of the parts in a single part file (probably want to investigate Sketch Blocks as well - since you have relative motion) and then push out the individual parts and assembly when completed (or nearly completed).

 

I will try to post an example tomorrow if I get a chance.  In the meantime - you should concentrate on getting correct fully defined sketches.

 

For the 35t chainring - do you want a true sprocket?  If so - I can walk you through an interesting proceedure that will give you a rock-solid understanding of parametric constraints and dimensions.


-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


EESignature

Message 18 of 38

JDMather: 

In order for me to manufacture something out on the shop floor - it should be fully defined.

So why shouldn't the designer do this work before sending to manufacturing?

 

I agree, the designer should be creating designs fully useable by the manufacturer. Do you mean that, the sketch I've created isn't fully defined, and by this, the nodes aren't properly intersecting so it's just a birds nest of lines? I've noticed that sometimes when I'm placing lines they aren't connecting properly. I'll have to be careful with that.

 

JDMather:

For the 35t chainring - do you want a true sprocket?  If so - I can walk you through an interesting proceedure that will give you a rock-solid understanding of parametric constraints and dimensions.

 

Thanks, but the chainring is only there as a dimensional tool. The aim of this project is to create the yoke which you have used in your attached image. It has to connect to the lower linkages and spread around the tyre without contacting the chainring. Everything else is merely there for my own learning or to dimension the yoke. My short term goal is to have the lower linkages and the yoke CNCed to build a new rear end for a test mule. My long term aims are to understand Inventor enough to be able to CAD from the groud up my own prototype frame (twhich has already been designed). The future prototype depends on the success of the suspension kinematics of this test mule. Unfortunarely, it's the yoke is the one darn thing I can't get right at the moment! I'll go back through your post and seek out tutorials and further learning on the areas you have mentioned, in the meantime, have you any ideas why when I try to extrude that part (see attached) I can only make a cut, and not a solid?

Message 19 of 38
JDMather
in reply to: oneloosecrank


@oneloosecrank wrote:
..I can only make a cut, and not a solid?

Walk out to the shop floor (figuratively - in your mind).

You have an assembly before you.  You can only cut existing parts.  You cannot magically add material.

 

Your sketch is at the assembly level - therefore it will only allow you to cut.

 

You need to create parts at the part level.

 

For your design - the easiest way to do this would be multi-body solids techniques.

 

Are you willing to start this one over from scratch?
Right from the beginning?

If so, I can walk you through how I would do the design.


-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


EESignature

Message 20 of 38
oneloosecrank
in reply to: JDMather

I see, if you are unable to add material in assembly then that explains a few things. I assumed that a new sketch would just start a new part - I did wonder why no new file was being created to go with that part...

 

And yes, I'm very willing to start over. There's a few dimensional short comings that I want to re-do as well. Advice on how better to approach project this is extremely welcome 🙂

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report