making a scissor lift

[michael_schmidlkofer]

I have an assembly that I have a base then I associate a rectangular plate with rounded ends that has 3 holes in it. One end goes to the base the middle goes to the rod where it is scissored to another plate and the second plate goes to another rod that is in a slide. Every time I try to associate the 3rd hole to the other rod the plate totaly disassociates with the other rod. (the plate is suppose to be free spinning)  What am I doing wrong?

[michael_schmidlkofer]

Every time I do an insert on one hole then I try to do an insert the hole in the middle it says there are interference. I have been starting over and I still have problems. According to what you put together. I should be doing inserts on the first hole then insert the second hole then insert the third hole. What am I doing wrong?

[michael_schmidlkofer]

You know all of your inserts have 0.000 offsets. For some reason I cannot duplicate it.

[michael_schmidlkofer]

is there really a video? I can't find it.

[michael_schmidlkofer]

how do you have both a Mate:3 and Insert:5 at sissor mar:2?

[michael_schmidlkofer]

Ok the only thing i need you to give me an answer for right now is sissor mar:3  you can see it  not where it is supposed to be. Middle hole is suppose to hook up to sissor or:3 middle hole. Every time I try it says "The assembly cannot be solved." I have tried everything to solve it. What do I need to do? Don't just solve it and say figure it out. I tried that. I couldn't figure it out.

[3D4Play]

I think I understand now. You don’t realize that you’re answering your own question. Watch my video, and note that I did not use insert constraints - I simply aligned two axes, and the beginnings of the assembly work fine under those constraints. Understanding the difference between an aligned mate constraint and an insert constraint will go a long way towards enlightenment and resolving your issues with that assembly. You shouldn’t have to dig very deep to see that the rod length relative to the space between the bars will prevent a second insert constraint from working in certain specific locations. That’s why I used an aligned mate constraint to demonstrate a solution. I hope that helps. 

[JDMather]

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@michael_schmidlkofer wrote:

 Don't just solve it and say figure it out. I tried that. I couldn't figure it out.

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@michael_schmidlkofer 

Are you ready to start over from scratch and do it right?

[michael_schmidlkofer]

it just takes me to your home page so where is the video and what is it called?

[JDMather]

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@michael_schmidlkofer wrote:

it just takes me to your home page so where is the video and what is it called?

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That doesn't answer my question.

Let me elaborate on my question, "If I give you step by step instructions on how to do this correctly, are you willing to start over from scratch to learn how to do all of this correctly?"

This is a binary yes/no response question.

[michael_schmidlkofer]

yes yes yes

[JDMather]

@michael_schmidlkofer 

If yes, 

STEP 1 Create a new project folder

Within this new project folder create a New Project and make sure it is active.

[JDMather]

STEP 2.

Start a new part file and then within the new part file start a New Sketch on the XZ plane.

Select the 2-Point Center Rectangle tool...

Sketch a rectangle centered at the Origin...

Add the dimension shown and then add an Equal (=) constraint between the horizontal and vertical lines as shown,

We will make use of symmetry about the origin throughout the design to make assembly easier.

[JDMather]

@michael_schmidlkofer 

Notice the "Thumbtack" on the Sketch1 glyph in the browser and at the lower right of the screen Inventor tells us that the rectangle sketch is Fully Constrained (defined - no ambiguity, robust and predictable).

[JDMather]

Go to the Right Side view and start a new sketch on the YZ plane.

Project Geometry the bottom line of the extruded rectangle from previous step.

Sketch two  2-Point rectangles as shown...

Dimension as shown below (remember the = sides constraint tip).

Extrude the Sketch2...

Mirror the extrusion to the other side ...

[JDMather]

We need to make an edit.

Right click on Sketch2 and select Edit Sketch.

Double click on the .125 dimension and change to .225 as shown..

Click on whichever line you made = and delete the = constraint.

Add the .125 dimension shown...

Do you see how we edited this feature more easily than you did in your original file?

[JDMather]

Go to the Bottom view on the View Cube.

Start a new sketch on the XZ plane.

Sketch a centerpoint rectangle as shown...

Finish Sketch.

Go to the Hole command and set as shown.

Click on the four corners of the rectangle.

[JDMather]

Go to the Front View.

Start a New Sketch on the XY Plane.

Hit F7 of the keyboard for Slice Graphics...

Project Geometry the short edge of the slot as shown...

Sketch a horizontal line from the midpoint of the projected line as shown.

Sketch a circle as shown.

Extrude-Cut symmetrically through all.

Attach your new file here for first set of assembly instructions.

[michael_schmidlkofer]

the = sign constrain says it is for circles.

[michael_schmidlkofer]

see attached

 

[JDMather]

@michael_schmidlkofer 

That is just an example.

Equal (=) constraint works for all entities of like types.

Circle1 = Circle2

Line1 = Line2