Spring pin problem

[jamami]

AF0001 A3 (1).pdf

 

For some reason I lost my very long message when I inserted the attachments!!!

In summary:

I have created the attached part using AutoCad both 2D and 3D.

I am now trying to use Inventor and have really struggled, I have completed the tutorials shipped with the program and have managed to create the pin body as attached (using a revolved sketch), but in doing so have a few questions.

1. How to use hole function to create the 3mm dia hole on the pin head, as it does not seem to like curved surfaces? (To achieve I extruded another solid and subtracted just like Acad)

2. How to align the emossed text exactly centrally, I have just eyed it in as constraint did not work.

3. How to find out the weight.

4. Is it possible to model the spring wire and clasp in Inventor? I have tried using a 3D sketch but there do not seem to be enough drawing tools (ie circle does not exist) to achieve this shape, also there do not seem to be snaps and grips etc. Do I have to do this in Acad and import?

5. How can I see my original sketch? It does not show up when I select edit or slice.

 

Any help much appreciated.

AF0001.ipt

Edited November 20, 2012 by jamami
Attachments wiped out original text.

[JD Mather]

1. Workplane tangent to cylinder. (see built in tutorials)

2. Dimension and constrain.

3. iProperties.

4. Yes you can do this (easily) in Inventor. What is this "Acad" that you speak of?

5. Expand feature in browser (click on + symbol next to feature) then right click no sketch and select Visibility.

 

You might want to go through the tutorials.

You might want to go through these tutials http://home.pct.edu/~jmather/content/DSG322/inventor_surface_tutorials.htm (especially the SkillsUSA document and Tutorial #7)

[jamami]

Thank you for your reply.

1/ I followed the built in tutorials but these did not help with the hole function on a curved surface. Does the hole function work on a curved surface? One of the example shows something similar by creating a hole from a point, but the trouble I have is locating the point accurately as there are no snaps on the 3d solid.

2/I middle and centre justified the text, but again the justification point did not appear for me to 'drag'. Are you suggesting I add a dimension to the text (height or width or diagonal?) or from the text to the object? Where would one add the constraint? I followed the glass bottle tutorial but this only helps with alignment in one direction, I tried to add a vertical constraint but received the message '...over constrained'.

3/I will investigate, thanks.

4/When you say 'easily' you are clearly talking from a personal perspective in the third person! Is it necessary to use a series of 2D sketchs or a single 3D sketch to model the wire centrelines? I assume it is simple path extrusion once complete? Apologies, Acad is a lazy way of saying Autocad.

5/Thank you.

[Bishop]

Thank you for your reply.

1/ I followed the built in tutorials but these did not help with the hole function on a curved surface. Does the hole function work on a curved surface? One of the example shows something similar by creating a hole from a point, but the trouble I have is locating the point accurately as there are no snaps on the 3d solid.

 

 

Create a work plane parallel to one of the origin planes, and tangent to the curved surface upon which you want to create your hole. Make a new sketch on this plane, and place a point on the center of where you want your hole to be. Finish the sketch, and start the hole feature. Create a hole from a sketch, and if it doesn't auto-select the point you created, then select that point and set your other options as appropriate. Your hole should appear.

 

 

2/I middle and centre justified the text, but again the justification point did not appear for me to 'drag'. Are you suggesting I add a dimension to the text (height or width or diagonal?) or from the text to the object? Where would one add the constraint? I followed the glass bottle tutorial but this only helps with alignment in one direction, I tried to add a vertical constraint but received the message '...over constrained'.

 

 

Turn off the text box and you'll get your point.

 

 

3/I will investigate, thanks.

 

 

More precisely, go into the iProperties for the part, and select the PHYSICAL tab. Your part mass will appear there, based on whatever material you've selected.

 

4/When you say 'easily' you are clearly talking from a personal perspective in the third person! Is it necessary to use a series of 2D sketchs or a single 3D sketch to model the wire centrelines? I assume it is simple path extrusion once complete? Apologies, Acad is a lazy way of saying Autocad.

 

He knows what ACAD is. He's suggesting - in a somewhat dry fashion - that you forget AutoCAD and everything about it. Inventor is not AutoCAD, and most of the ways that you did things in AutoCAD aren't going to work the same way - or even close to the same way - in Inventor.

 

Yes, you'll need a series of 2D sketches to get the path you need. Without trying it myself, I'd say ... 2 or 3 sketches. You could do it in 2, I think, but it'd be awkward to get some of the geometry right. The first way that I'd try it would be 3. The first one would have a surface extruded out of it, and the second and third would be projected on to the surface. (You could skip actually extruding the surface, but I find it helpful for visualizing what I'm doing.)

 

Anyway, I'd also only create one half of the spring thingy at a time with the sweep operation, and then I'd mirror that half to create the other half.

[JD Mather]

...He knows what ACAD is. He's suggesting - in a somewhat dry fashion - that you forget AutoCAD and everything about it.....

 

at least someone understands my dry attempt at humor....

[JD Mather]

I recommend that you go back and read that SkillsUSA document from the url I posted earlier.

Your Sketch1 is not constrained.

Worry about this now, and later on you won't have to because Inventor will be creating all these constraints for you.

 

 

Now you didn't really need 4 dimensions, but use the BORN Technique and also leave 45° chamfers and fillets out of sketches - add them as features.

 

[Bishop]

spring clip.ipt

 

 

This is how I'd do it.

[JD Mather]

First add a horizontal or vertical dimension to the text box as appropriate.

then

right mouse button turn the box off and you will see a centerpoint grip that you can dimension or constrain

but

I usually just add a dimension to the text box (size doesn't matter) and then sketch a diagonal construction line to use the midpoint for constraining.

 

[JD Mather]

This is how I'd do it.

 

Very nice work!

 

Just add a cut in the ends where they go into the hole in the pin.

 

Noticed a bit more missing - but your file should give the OP a good idea how to continue.

 

Edited November 20, 2012 by JD Mather

[JD Mather]

jamami

 

instead of extruding a circle for the hole - simply place a sketch point to use with the Hole command.

I would create a sketched line from the origin to center the point and then add one dimension to position.

[Bishop]

Very nice work!

 

Just add a cut in the ends where they go into the hole in the pin.

 

Noticed a bit more missing - but your file should give the OP a good idea how to continue.

 

 

 

Thanks. I wasn't going for exact accuracy from the drawing, just a basic idea of how to do it. To be honest, I didn't even look at the drawing - just the 3D model from the OP.

 

Also - are you going to be in Vegas next week JD?

[JD Mather]

Also - are you going to be in Vegas next week JD?

 

No - can't go this year.

[jamami]

Thanks for the excellent advice and input. My first day of inventor has been an interesting one.

I will study your attachents and the tutorials, but I cannot promise not to ask more basic questions.

Thanks again.

 

PS I did get the Acad point, I was my attempt at oblique reciprocation

[jamami]

and place a point on the center of where you want your hole to be.

 

I need the hole to be mid way through the pin head, ie 3mm from either the top or bottom. Do I draw the point or circle at any location and then dimension or constrain to mid point? I cannot get the cursor to snap to anything( I assume this is intentional to force explicit point creation?)

[jamami]

Thats really neat, I havent managed to complete myself but will persevere. How many 2D sketchs did you need? What is the purpose of the 3D sketch option? First appearances would suggest this is a true 3D problem.

 

There is a clasp to hold the spring wire together at the tip of the V profile, this is a sheet metal part (T shape) pressed around the spring wire. What is the best way to deal with this? Draw as a sheet metal part? How can the geometry of the parallel wires be extracted to form the inner profile of the clasp? Or is it a case that from knowledge of the wire diameter the componet is drawn in the 'final' position?

 

The completed pin consists 1xbody, 1xspring wire &1xclasp. Do I prepare individual ipt files for each part and then join together in an assembly file?

[jamami]

Thanks for text box tip, I have managed to complete this now. Regarding the 2D sketch why does specifying dia12 and dia16 provide anymore constraint than detailing 6 and 8 resp half sizes?

[Bishop]

I need the hole to be mid way through the pin head, ie 3mm from either the top or bottom. Do I draw the point or circle at any location and then dimension or constrain to mid point? I cannot get the cursor to snap to anything( I assume this is intentional to force explicit point creation?)

 

 

You're still thinking AutoCAD here ...

 

You -can- snap to things, but there has to be something to snap -to-, and it doesn't always work the way that you're expecting it to. You can play with some of the options in TOOLS --> APPLICATION OPTIONS --> SKETCH. Take a look at the part I've attached here. The construction line that the point is constrained to was made using PROJECT CUT GEOMETRY, and it represents the line where the work plane is tangent to the face of the cylinder. Since it's only just the length of the cylinder, I've got a midpoint there that I can constrain the point to.

 

 

hole in cylinder.ipt

[Bishop]

Thats really neat, I havent managed to complete myself but will persevere. How many 2D sketchs did you need?

 

I used 3 2D sketches to create the sweep path, plus a 4th to provide the circle that I swept around the path.

 

 

What is the purpose of the 3D sketch option? First appearances would suggest this is a true 3D problem.

 

It is a 3D problem ... but sometimes the quickest way to create 3D stuff is to start from 2D references.

 

In the sample I uploaded, Sketch 1 creates the overall shape along the YZ plane. Sketches 2 and 3 are projected onto that shape in the positive and negative Z directions, respectively. The 3D sketch is created by projecting the intersections of Sketch 1 with Sketches 2 and 3. This gives us our 3D profile to follow.

 

There is a clasp to hold the spring wire together at the tip of the V profile, this is a sheet metal part (T shape) pressed around the spring wire. What is the best way to deal with this? Draw as a sheet metal part? How can the geometry of the parallel wires be extracted to form the inner profile of the clasp? Or is it a case that from knowledge of the wire diameter the componet is drawn in the 'final' position?

 

What is the clasp going to be made out of? Is it stamped or cast or what? If it's cast, I'd create it as a separate solid, use combine with keep toolbody checked to cut the wire shape out of it. If it's stamped ... I'd still probably create it as a separate solid, but I might do it as a surface body that i'd then thicken and derive out as a separate part. I don't know - hadn't thought that far ahead yet.

 

The completed pin consists 1xbody, 1xspring wire &1xclasp. Do I prepare individual ipt files for each part and then join together in an assembly file?

 

 

Yes.

 

Now, what you might wind up doing is modelling it all as a single .IPT file with multiple solids. If you do that, just bear in mind that it's NOT an assembly. You'll still want to use MANAGE --> MAKE COMPONENTS and then generate separate .IPT's for the solids and put it in an assembly.

[Bishop]

Thanks for text box tip, I have managed to complete this now. Regarding the 2D sketch why does specifying dia12 and dia16 provide anymore constraint than detailing 6 and 8 resp half sizes?

 

 

Not sure that it does. I think it might be just a style thing as much as anything. What JD did there was set the one edge as a centerline, and then when he dimensioned from it to the outside, Inventor assumed that it was a diameter, to be symmetrical across the centerline. I've never actually done that before, myself, but there's a reason why he's a professor and not me. To be perfectly honest, I didn't even know that would happen!

[jamami]

Its hard not to think of, shall we say, 'the other application'. Only been 1 long day on Inventor so far, most of which has ben spent reading JD's tutorials, looking at your examples and looking through the forum. Your input has been excellent and I really appreciate it. I promise never to mention 'the other application' again.