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How to derive a part from two other parts (sketches)

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Message 1 of 13
mechamania
896 Views, 12 Replies

How to derive a part from two other parts (sketches)

Hi

 

I often use a number of parts with only one sketch in them as templates for other parts.

I have for instance a template part with a top view sketch and a template part with a side view sketch.

Mostly I can use one of these template parts to derive my parts.

But now I want to creat a part that needs both the top view and side view sketches. So I need to derive from

two different parts.

 

How can I do that?

12 REPLIES 12
Message 2 of 13
torbjorn
in reply to: mechamania

First, I don't really understand your workflow, It would be interesting if you could elaborate some on the intensions of this workflow. 

 

When thats saild, I believe you can derive as many parts(or anu of its sketches, planes, workfeatures etc) as you want into a single part. But of course, they will be placed as defined by the coordinate system of the derived part.

Message 3 of 13
JDMather
in reply to: mechamania


@mechamania wrote:
How can I do that?

Use the Derive Component command.
Attach your files here if you can't figure it out.


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Message 4 of 13
mechamania
in reply to: JDMather

My workflow is as follow:

 

I make a sketch containing the top view items of my product. This sketch is saved in a part file (template_top.ipt).

I also make a sketch containging the side view items of my product. This sketch is saved in another part file (template_side.ipt). So these two files contain my template sketches.

 

Then I make the derived parts (using the' Make Part' function inside the template parts). Normally I only need one of the

templates to create a new part.

But now I have a situation where I need both template (the sketch in template_top.ipt and the sketch in template_side.ipt) to create the part. As I understand you can only derive from one part. But I need to derive from two parts. Can that be done?

 

I hope this explains it a little bit better.

 

Message 5 of 13
JDMather
in reply to: mechamania


@mechamania wrote:

... (template_top.ipt).

...(template_side.ipt).  

Then I make the derived part


Attach these 3 part here.

 

Derive Component.png


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Message 6 of 13
mechamania
in reply to: JDMather

@ JDMather

 

I have no access to the computer at this moment. I will have later today.

Can you tell me how to do it so that I can try it myself?

Do I have to use the 'Make Part' to create the derived part and then somehow add another part (second template part) 

to it? If so, how do I add the second one?

 

 

Message 7 of 13
JDMather
in reply to: mechamania

I am too curious about your workflow to attach the solution just yet (it is trivially easy) but I can't figure out why you are doing what you are doing.


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Message 8 of 13
mechamania
in reply to: JDMather

Here is an assembly containing several parts that uses a template sketch. In this case there was one template.

 

 

Message 9 of 13
JDMather
in reply to: mechamania

I thought I might learn something - but I am totally confounded by your workflow.

 

Why don't you use multi-body solids?

Why do you put so much into one sketch (in my experience it is better to create many sketches)?

I would at least hve to use more Equal (=) constraints to remove duplicate dimensions.

Why would you need a different view sketch in a completely different file?

 

Now to answer your question.

Make Part is a relatively new addition to Inventor.

Make Part pushes out a Derived Component.

 

The old way was to start a new file and Derive to pull in the derived geometry.
so

simply go ahead and Make Part to get started and then in the resulting file click Derive to pull in the second file.

 

Derive.png

 

 


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Message 10 of 13
JDMather
in reply to: JDMather

While I have this one up on my screen - your assembly will not work in the real world.

You have not allowed clearance for motion and manufacturing tolerances.

Even if we could make perfect parts - a 86mm yolk will not rotate about 86mm bearings.
A 25mm cylinder will not rotate in a 25mm hole.


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Message 11 of 13
mechamania
in reply to: mechamania

Thanks.

 

I do not have much experience with good CAD practice. So I'm open to any suggestion.

And the files I did attached are just ment for proof of concept. It will not be produced this way. So I did not bother

to have correct tolerances in it.

 

The reason I put more parts into one sketch is to be able to relate the sizes of different parts to other parts.

This is the idea behind templates, isn't it? I agree I should use more =(equal) constraints.

And I agree that it would be better to put both sketches into one part file. I did think of that to late. I already had a lot of

templates sketches drawn. I think it is difficult to put them into one part file now, because I have to redo all derived parts.

 

I will study the multi-body part feature. I'm not familiar with that at the moment.

 

Thans for the solution.

 

Message 12 of 13
JDMather
in reply to: mechamania


@mechamania wrote:
 

The reason I put more parts into one sketch is to be able to relate the sizes of different parts to other parts.

 


You can still do this with multiple sketches. I have a general rule of around max 7 entities in a sketch.'
You can Project Geometry from one sketch into another to tie together sketches (project only what is needed).

And name dimensions so that the parameters can be used between sketches.


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Message 13 of 13
mechamania
in reply to: mechamania

Thanks for the tip!

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