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: 

Wow, is this tutorial meant to be so challenging?

24 REPLIES 24
SOLVED
Reply
Message 1 of 25
ross350
1512 Views, 24 Replies

Wow, is this tutorial meant to be so challenging?

Hi,
This looks like a pretty helpful forum, I've got an idea and I'm trying to make it in inventor2014..
I want to make a prototype using dovetail joints where suitable, I can cut and plan them with pen and paper, or mark the wood directly but I'd like to use a tool to make a proper plan including the joints and I found this tutorial that let's you make a tool to makes the joint parameters change, I think I could use this tool quite allot but the tutorial is leaving me with open loops on the side pins when I go to extrude the sketches.
Could someone take a look at it and give it a go making it? I'd be very grateful if you could send me the completed tool or even tell me some things that might be missing from the tutorial.
Thanks
24 REPLIES 24
Message 2 of 25
ross350
in reply to: ross350

Message 3 of 25
JDMather
in reply to: ross350


@ross350 wrote:
... the tutorial is leaving me with open loops on the side pins when I go to extrude the sketches.

Attach your *.ipt file here.

I don't want to speak for Steve, but when I write a paper like that it is intended to be limited notes for those who attend the presentation. A suppliment to the class, not a replacement. Before teaching/learning iParts I would expect the user to have significant prior experience and be able to create any required sketch.  This would  be an intermediate to advanced level class.

 

Attach your part and someone will show you how to fix it.


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


The CADWhisperer YouTube Channel


EESignature

Message 4 of 25
ross350
in reply to: ross350

Hi,
I only sat down and really tried to use inventor for the second time today and I know this is a pretty sophisticated itool.
I am berry determined to master the use of this particular tool and I will make up a new file, following the instructions and post it here tomorrow. Thank you
Message 5 of 25
ross350
in reply to: ross350

Very*
Message 6 of 25
JDMather
in reply to: ross350


@ross350 wrote:
Hi,
I only sat down and really tried to use inventor for the second time today ....
...

Create your new attempt and attach it here tomorrow, but I recommed you go through these before trying to do too much and developing bad (for Inventor) modeling habits.

http://home.pct.edu/~jmather/SkillsUSA%20University.pdf
http://inventortrenches.blogspot.com/p/inventor-tutorials.html
http://wikihelp.autodesk.com/enu?adskContextId=HELP_TUTORIALS&language=ENU&release=2014&product=Inve...


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


The CADWhisperer YouTube Channel


EESignature

Message 7 of 25
Curtis_Waguespack
in reply to: ross350

Hi ross350,

 

So the tutorial you linked to is a bit out of date in terms of the tools that were available when it was written. Attached is an example file that demonstrates a very simple dovetail joint made using multibody solids in a single part, and using the Combine tool to subtract one solid from the other. Use the End of Part marker to step through the part to see how each feature was created. Note that once the joints are create, you could write each solid out as an individual parts useing the Make Components tool. You could also, use the Thicken/Offset tool to loosen up the joints to add some fit tolerance.

 

Also, have a look at this link and I think you'll see some familiar issues that you've encountered already:

http://inventortrenches.blogspot.com/2011/03/inventor-101-simple-fully-constrained.html

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Message 8 of 25
ross350
in reply to: ross350

That is so helpful, THANKS!

I've put the file I was working on, please take a look and let me know why those sketches wouldn't extrude properly.

I probably would work it out by following some of the links reccomended to me, so I will try those soon.

 

I just get the feeling it might be something in the settings because they are pretty much stock settings.

I'd like to be able to show that all dimensions are, what is the setting for that because when I push F8 like I read somewhere it doesn't show anything.

 

thans again,

 

Message 9 of 25
JDMather
in reply to: ross350

Sketch1 is missing a dimension and not placed at the Origin Center Point (most basic of all Inventor techniques - master this).

(and it is easy - as Inventor will do it for you - simply click on the projected origin as your first point when creating the rectangle) 

 

Workplane1 is not needed because the step above was not done correctly - more extra work that Inventor would do for you.

 

Sketch2 is missing a dimension.  The width dimension is not needed as it has already been defined.  The 90° dimension is not needed as it has already been defined.  Actually - all of Sketch2 is not needed (even though it is used in the original tutorial - I'll explain later.

 

Sketch3 and 4 have no apparent purpose and can be deleted.

 

I will explain step-by-step corrections.


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


The CADWhisperer YouTube Channel


EESignature

Message 10 of 25
ross350
in reply to: Curtis_Waguespack

Hi.

just a follow up, on that file you sent.

I made a set of user defined parameters,length,width,thick,Tailwidth,Tailslope and pitch,

then I attmepted to adapt the model you sent to those parameters so I could change a few measurements but keep usable plans for the joints,

Thats my main focus here, and you model worked mostly.. 

but now I want to know why a few things didn't go so well and I have attatched the file after my attempt so you can see what I mean.

1:Why doesn't Extrusion3 have a dimension I can change for it's Y axis? (I've named it "width" in extrusion1 and could change that one)

2:Extrusion1 has a dimension (d4) that I just cant work out how it works, it makes your model a little bit different to the one in the tutorial, doesn't it?

 

Message 11 of 25
ross350
in reply to: JDMather

Thank you,

when you say "projected origin" do you mean the centre dot that is at the 0 point on a blank new window?

I will try again to start a new one from scratch right now and post it up when done

Message 12 of 25
JDMather
in reply to: ross350

Yes, that is what I mean.

After we go through this - you will see that it is trivially easy once you know what you are doing.


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


The CADWhisperer YouTube Channel


EESignature

Message 13 of 25
ross350
in reply to: JDMather

ok,

I have just started and I want to work something out.

I make a rectangle 2 different ways,

1/The first way is just drag out a 2 point centre rectangle and place it with the mouse at the measurements I want.

something I notice when i do this and then later want to set up parameters, I cant get the Height (z axis in the attached file REV1)

It gets reall stange and give me a wacky angle at the top..

 

the second way is , I start the 2point centre rectange with a click and then key in the desired dimensions manualy,

This lets me keep those dimensions and so I can set up parameters linked to those measurments... which is vital for what I want to do with these joints..

 

in the first scenario if I use the dimensions tool in /sketch and put in a measurement longways on that rectangle, I get a driven dimension.

I can't change a driven dimension, so I am stuck.. 

 

I know to do it the second way and that will prevent any problems, but what is a curative remedy for this kind of problem, incase I find out later in the process or as my previous post outlined where I couldn't find the dimension for the other piece of the join he uploaded.

 

I really appriciate the help. 

 

Message 14 of 25
JDMather
in reply to: ross350

Rev1

This angle dimension is completely meaningless.

Right click on the sketch in the browser and select Edit Sketch.

Then click on this dimension and delete it.

You do not care what that angle is.

The only thing you care about is the width and height of the rectangle.

 

Angle dimension.PNG


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


The CADWhisperer YouTube Channel


EESignature

Message 15 of 25
ross350
in reply to: JDMather

I'm sorry, I didn't mean to say this was solved..

https://www.youtube.com/watch?v=XkJ5GmP-ksE
this movie shows the tool I want to make, and can make following these instructions
http://www.widom-assoc.com/MA319-5_The_Sharpest_Tool_For_Woodworking.pdf

if it's so easy then could you show me a working example of this tool.
in a file please.
Message 16 of 25
JDMather
in reply to: JDMather

Go to the Top view and start a New Sketch on the top face.

 

Select Project Geometry and click the edge shown.  (My guess is that you did not read the document I linked earlier - in which case Inventor already projected this edge - so you can skip the Project Geometry if it is already projected.)

 

Project Geometry.PNG


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


The CADWhisperer YouTube Channel


EESignature

Message 17 of 25
JDMather
in reply to: JDMather

Sketch a horizontal line being sure to select the midpoint of the vertical line as the first point of the line.

Window select all of the lines and click the Construction icon as shown.  This will convert your lines to dashed construction lines.

 

Construction Lines.png


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


The CADWhisperer YouTube Channel


EESignature

Message 18 of 25
JDMather
in reply to: JDMather

Sketch the short vertical line in space close to the short horizontal line as shown.

 

Vertical line.PNG


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


The CADWhisperer YouTube Channel


EESignature

Message 19 of 25
ross350
in reply to: JDMather

The big question is where in revA is the Z axis projected to? because it isn't showing up for me can you find out,

And then in that same file I want you to type 3000mm into user parameters with the word (BIGGER) and then I want you to the sketch and change the

Z axis measurement of that rectangle to the user parameter just by using the word BIGGER.

I want you to simply do that and send me the edit, maybe then I can see 

 

 

Message 20 of 25
JDMather
in reply to: JDMather

Select the Coincident Constraint icon and click the midpoint of the vertical line and the endpoint of the horzontal construction line as shown.

 

Coincident.png


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


The CADWhisperer YouTube Channel


EESignature

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

Post to forums  

Autodesk Design & Make Report