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Seemingly simple constraints in an assembly being impossible to implement


HCb

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There are certain "faults with my Sketch1 that I can't seem to resolve, ...

 

You are missing a Vertical constraint on your "vertical" line

and

the right endpoint of the arc is drawn to the wrong location (go back and check previously posted images).

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  • JD Mather

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JD, thank you for your help (sorry, I may overload with the thanks but I know it takes time to do what you're doing and it is appreciated).

 

I opened my drawing up and I do not see a thumbtack on either of my sketches in the Browser. Fearing I may have modified the drawing after posting it here (not really likely) I downloaded the drawing file I posted here but see the same results; there is no thumbtack on my Sketch2 (or Sketch1).

 

I modified the drawing as you suggested, moving the endpoint of the construction line to the endpoint of the arc at the eye of the spring. I agree with your philosophy of catching every detail possible and it's how I do things in my shop; there's always plenty I'll miss, I better nail everything I can think of perfectly to minimize the failures from the stuff I'll miss. Anyway, I agree, and I've modified the drawing accordingly and it looks neater (cleaner) for it. However, after the program tells me the sketch is Fully Constrained, I still do not have a thumbtack in the Browser (yes, I clicked Finish Sketch). I'm not telling you how it is with this statement, just telling you what I thought: I thought that the thumbtack meant the sketch was anchored (constrained) to the origin of the sketch plane. I'm probably nit-picking but I hate to miss a detail which may be important and I do not have a thumbtack on either of my sketches in the Browser though both sketches are Fully Constrained.

 

Thanks again.

 

Moving on to the next post.

 

--HC

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Here is image of my two finished sketches with dimension display turned off. I normally don't turn off dimension display unless the dimension are set in stone (won't change). If a dimension does need to be changed it is a simple matter of double clicking on the dimension.

[ATTACH=CONFIG]45806[/ATTACH]

I could have eliminated all but one of the Thickness dimensions by using short vertical lines from the end of the original vertical line and then making them Equal (=) constraint. That is what I would normally do for something like this. This would be a good challenge for you to figure out (actually pretty simple).

 

I'm sorry, JD, I missed the detail of you asking for a post of the file after the continuation of the arcs. I am posting the resultant file both with the offset of the previous arc projection and with short construction lines set equal to the first short line (actually, I set each short line equal to the one above it; a seemingly small/insignificant difference).

 

--HC

 

Circle and line for JDMather rev 3a.ipt

Circle and line for JDMather rev 3b.ipt

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Extrude each sketch midplane (symmetric) 2" (because the profiles are open you will have surface bodies.

After doing the second Extrude you will have to expand the ExtrudeSrf2 feature and right click on Sketch2 and select Visibility.

 

After extruding the surfaces then Thicken each one by Thickness (for the first Thicken set to Quilt since it is multiple surfaces).

Be sure be sure be sure to set as New Solid for each Thicken (after the first one).

 

 

[ATTACH=CONFIG]45809[/ATTACH]

 

Right click on the Surface Bodies folder in the browser and turn off Visibility.

Add you fillets to each solid body.

 

Thank you. Attached is the file as it stands at this point. Quite a different approach than what I was trying and it works well, thank God.

 

--HC

 

Circle and line for JDMather rev 4.ipt

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Turn the visibility of Sketch1 back on and start a new sketch on the XZ Plane.

Select Project Geometry and then the vertical line from Sketch1.

Add a (sketch) Point at the projected point.

Hit H on the keyboard to start the Hole command.

 

Select all of the solid bodies to drill holes Through All.

Set you desired hole diameter.

 

[ATTACH=CONFIG]45810[/ATTACH]

 

Turn off visibility of the Sketch1.

Post back for instructions on how to convert this multi-body solids file to an assembly if desired.

 

JD, thanks again. Finally done. File is attached.

 

Since this part is all one part and not an assembly of individual parts, what would be the significance of creating an assembly from it? I don't mean that as a rude challenge, I simply do not understand how making it an assembly would change how I use it in my overall assembly file.

 

I'll try to convert it to an assembly but my first thought would be to simply create an assembly file and populate it by placing this one part in it.

 

--HC

 

Circle and line for JDMather rev 5.ipt

8K Spring.zip

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Oops, I forgot that you are using an old version of Inventor. I guess the thumbtack image to sketch was not added till later version, but in lower right corner of screen it should tell you when the sketch is fully constrained.

 

If you have no real reason to convert this to an assembly then it is not necessary to do so - simply place it as a component in your master assembly.

But for assembly BOM and individual part drawings some situations might require that you have this exactly like it is in the real world - that is a part is a single part and an assembly (or subassembly) is a collection of parts. If you needed to push this to an assembly that would be accomplished by going to the Manage tab and using the Make Components tool (and following the on-screen prompts).

 

There are a couple of other considerations in this design.

Earlier I told you that the dimensions were not manufacturable (especially for something low tolerance like a spring).

 

Arcs with radii beyond 3 decimal places on a design like this are not really manufacturable - we eliminated those.

But angle dimensions are also difficult to control.

 

For Design for Manufacturability considerations I would -

1. change the angle dimensions to Reference (select and then Reference in upper right corner of sketch screen) and replace with reasonable arc length dimensions (round off probably to .1 or maybe .01) this will change the angles slightly, but they are only for reference.

 

2. This brings up a second (and third?) problem in that if we use arc length dimensions (this gives us what would be the flat length of the spring (other than first leaf) we should Thicken mid-plane instead of to one side. If we thicken to mid-plane we need to make half thickness allowance to the hole loop on the left end so that it ends up correct size. (we might also consider bend allowance (material compresses on the inside of a bend and stretches on the outside) but I think that would be overkill on a non-precision parts assembly like this.

 

3. Your first leaf is not of uniform thickness because you used the wrong size fillet(s) on the right end. Early on I was thinking I would show you how to use Inventor Sheet Metal tools to take care of this automatically, but decided not to introduce that just yet.

 

Thickness.png

 

Everything we have done could be done exactly the same way in AutoCAD.

 

Students can download Inventor 2014 for free here http://www.autodesk.com/edcommunity

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By the way - you could have done this all in 1 or 2 sketches rather than 6 sketches. (for the leafs and then the sketch for the hole)

 

There is a way to make the spring flex like a real spring, but that is an advanced topic.

(find the Scissors Inventor Sample (might have to download) for information on a similar Adaptive spring)

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I wish to thank you Dr. Mather for this tutorial.

 

 

After a rocky start I completed the spring assembly and learnt a great deal doing it.

 

 

There was only one hiccup, when offsetting arcs for the various leafs it offset the arc and the two construction lines leading to the arc centre. I tried several methods but settled on offsetting the original arc from sketch 1 and then drawing in the construction lines back to the centre. Changed the angle and it was good.:)

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Raygers, see attached screen shot of offset command. For hiccup referenced, try right clicking after you select offset command and make sure "loop select" is unchecked (mine is checked here). Now you should be able to click on individual entities. Once you have everything you want selected right click again and select "continue".

 

Offset.jpg

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Oops, I forgot that you are using an old version of Inventor. I guess the thumbtack image to sketch was not added till later version, but in lower right corner of screen it should tell you when the sketch is fully constrained.

 

If you have no real reason to convert this to an assembly then it is not necessary to do so - simply place it as a component in your master assembly.

But for assembly BOM and individual part drawings some situations might require that you have this exactly like it is in the real world - that is a part is a single part and an assembly (or subassembly) is a collection of parts. If you needed to push this to an assembly that would be accomplished by going to the Manage tab and using the Make Components tool (and following the on-screen prompts).

 

There are a couple of other considerations in this design.

Earlier I told you that the dimensions were not manufacturable (especially for something low tolerance like a spring).

 

Arcs with radii beyond 3 decimal places on a design like this are not really manufacturable - we eliminated those.

But angle dimensions are also difficult to control.

 

For Design for Manufacturability considerations I would -

1. change the angle dimensions to Reference (select and then Reference in upper right corner of sketch screen) and replace with reasonable arc length dimensions (round off probably to .1 or maybe .01) this will change the angles slightly, but they are only for reference.

 

2. This brings up a second (and third?) problem in that if we use arc length dimensions (this gives us what would be the flat length of the spring (other than first leaf) we should Thicken mid-plane instead of to one side. If we thicken to mid-plane we need to make half thickness allowance to the hole loop on the left end so that it ends up correct size. (we might also consider bend allowance (material compresses on the inside of a bend and stretches on the outside) but I think that would be overkill on a non-precision parts assembly like this.

 

3. Your first leaf is not of uniform thickness because you used the wrong size fillet(s) on the right end. Early on I was thinking I would show you how to use Inventor Sheet Metal tools to take care of this automatically, but decided not to introduce that just yet.

 

[ATTACH=CONFIG]45829[/ATTACH]

 

Everything we have done could be done exactly the same way in AutoCAD.

 

Students can download Inventor 2014 for free here http://www.autodesk.com/edcommunity

 

Hey, JD, yes, an older version. I got an educational license and it's good for awhile. I seem to remember seeing the thumbtack but maybe that's been in screen shots from others (and/or you)?

 

I don't use my drawings (2D currently) to track my parts I buy; I usually keep that in a text document in the project folder so I don't know why I'd need this to be an assembly in regards to parts tracking. I am not trying for a job in a design shop where it would be necessary. I'm doing this for me to supplement and improve what I currently do and it's a one-man operation.

 

I am re-drawing over and over this assembly. I'm doing it without reading this thread to try to make myself remember how to do it. In the process I will look at the dimensions and arc lenhths.

 

I would like to know more about the Sheet Metal tools. I've read somewhere that one can "un-roll" a shape to get the 2D representation. I would like to be able to model two pipes of whatever size and join them and then get a template for the saddle on the terminating pipe. I once wrote a VB6 program to print a sinusoidal form that I could trim and physically wrap around the pipe to mark the saddle cut. Yuck. It would be great to get that from Inventor. That's a topic for another day.

 

My fillets are not correct, yes. But the overall shape is close enough (for the whole part) to do what I need which is to plan for the height of the goose neck hitch so it will interface with my truck. Since the part won't be manufactered from this drawing I'm not going to sweat that.

 

I'll also play with the different thickening offsets. I've got a long way to go and, like I said, I'm doing this part over and over to try to get better. I'll experiment as I do that.

 

I will go back and re-visit AutoCAD for this. I would like to buy just one of the programs and if AutoCAD (not LT) will do the 3D that I need then that'd be great. I can use DraftSight for 2D and buy SolidWorks or Inventor, but I really like AutoCAD and feel comfortable with it so it it can do both for me then that might be the best place to spend the money. I've not been thrilled with AutoCAD's 3D so far but 1) I don't have much experience with it so it may not be a shortcoming of AutoCAD and 2) I'm using a laptop with perhaps a crappy video card for running 3D on AutoCAD (though I have no problems with Inventor).

 

I'm no longer currently enrolled as a student so I'll have to keep what I have for now until I make a purchase decision.

 

Thank you for all your help and time. I'm sorry if all this doesn't make much sense; I was up past 3 AM re-doing the spring drawing and then my son woke us up at 7...I'm running on fumes.

 

--HC

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I wasn't sure if I should try to do it as one sketch. Like I said in my last post, I'm re-doing this drawing over and over to try to get more proficient and to make sure I remember how (without reviewing this post; I'm doing it from memory or trying to, anyway). I'll try that, too.

 

At this time I don't have any desire to try loading the springs to see how they flex. Since I'm not designing the actual springs (I'll just be buying commercially-available items) it doesn't seem necessary (not meant to sound like I have a bad attitude, just simply a fact and I have years experience building trailers with success...I just need to determine the ride height of the trailer and it's good to draw the springs for experience).

 

I will play around with some movement constraints for the fun of it and to learn. I have tinkered with getting the springs to move around on the hangers and the equalizer to see how it will work over rough terrain. Now that I'm getting the springs dialed in I'll get to work more on that.

 

Still running on fumes... :-/

 

--HC

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