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Trim doesn't

9 REPLIES 9
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Message 1 of 10
rickduley
3393 Views, 9 Replies

Trim doesn't

I am doing JDMather's Surface Caps tutorial - modelling a screwdriver.  I don't have the file "Screwdriver Handle Toolbody.ipt" he refers to so I have tried to recreate it.  I guess I'm just not as good as JD Smiley Surprised

 

_Handle_Grip_Profile.jpg

 

In the IPT attached I want to be able to Trim the parts of the small circles inside the big circle, and the bits of the big circle inside the small circles.  Trim will let me do the latter, but not the former.

 

Why is this?

 

All assistance appreciated.

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9 REPLIES 9
Message 2 of 10
-niels-
in reply to: rickduley

It will not let you do the former because you've made the small circles as an associative pattern.
You can either edit the pattern and remove the associativity or trim the circle before you make the pattern.
But depending on the way you're going to use the circle, it might be better to make the pattern as a feature outside of the sketch.

Niels van der Veer
Inventor professional user & 3DS Max enthusiast
Vault professional user/manager
The Netherlands

Message 3 of 10
admaiora
in reply to: rickduley

I don't know the tutorial that you named.

 

But just some point:

 

- with some exceptions i tendencially avoid the trim command in the sketch enviroments, don't think as you do in Autocad. When you trim often you lose constraints and gain degrees of freedom of the geometry

 

- in this case you can't trim because you use the 2d serie in the sketch

 

- I prefer pattern the 3d feature instead the 2d geometry in the sketch

 

- if you want to do that anyway you can pattern your circle already trimmed

 

 

 

JD centanly will answer soon more accurately about his model.

 

 

Admaiora
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Message 4 of 10
JDMather
in reply to: -niels-


@-niels- wrote:
...
But depending on the way you're going to use the circle, it might be better to make the pattern as a feature outside of the sketch.

Follow niels' advice. 

I didn't know how to use Inventor back when I wrote that tutorial.

Pattern Features rather than sketch entities.

 

 

 Really, only two dimensions are needed in a simple sketch.

(image is from a Fusion 360 sketch)

 

Two dimensions.PNG

 

 


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Message 5 of 10
rickduley
in reply to: -niels-

Thanks niels, that solved the trim problem but I still can't get the extrusion to work.  I tried JD's sketch but that doesn't help much.  I guess I just don't understand what you mean when you say, "...  it might be better to make the pattern as a feature outside of the sketch."  I thought sketches become features when you extrude them.  Would you please explain in a bit more detail.  Thanks.

 

BTW JD:  If it only took you from 2006 to now to learn Inventor, there's hope for people like me yet Smiley Happy !

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Message 6 of 10
JDMather
in reply to: rickduley

It is rather astonishing how different your model (especially Sketch12?) is from my example considering the image I attached above.

Give me a few minutes to fix up the part - I'll be back.

 

Only took a couple of minutes to recreate this sketch.

 

Sketch1.png


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Message 7 of 10
JDMather
in reply to: JDMather

Oops, I realized that you switched to metric dimensions of a different size.

You should be constraining EVERY sketch.

You should not need to create ANY workplanes for simple geometry.

 

Try the attached file.

 

The idea is to create the extrusion and the Circular Pattern the extruded feature rather than pattern the sketch.


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Message 8 of 10
rickduley
in reply to: JDMather

Hi JD

 

I am afraid that your last sentence ("The idea is to create the extrusion and the Circular Pattern the extruded feature rather than pattern the sketch.")  is not grammatical.  I cannot understand what you are saying. Would you please clarify.

 

Thanks

Message 9 of 10
JDMather
in reply to: rickduley

1. Create the Extruded feature.

 

Extruded Feature.PNG

 

2. Create a Circular Pattern of the Extruded feature.  (6 copies in 360°)

 

Circular Pattern of Feature.PNG

 

 

The alternative would have been to pattern the sketch entities as in the original example.

But pattern sketch is not efficient as pattern feature in most cases.

Try this experiment, on your file with the pattern sketch - right click and select Show All Constraints (actually you left out a bunch of constaints) solving all of those sketch constraints really slows down a file.

 

If it looks too complicated - it probably is.

Sketch Constraints.PNG

 

 

Here is how I should have done the sketch.

 

Efficient Sketch.PNG


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Message 10 of 10
rickduley
in reply to: JDMather

Well, I finally got there.  Smiley Happy

Screwdriver Handle.jpg

 

Trouble is, I only got there by slavishly copying JD's dimensions and constraints.  Consequently, I learnt nothing except that JD could do this.  I am still all at sea about the underpinning theory in use here.

 

Apparently there is no User Manual for Inventor 2015, not even an on-line one, and I haven't found a tutorial which will give me an answer (perhaps there's something amongst the ones on YouTube but I become increasingly disenchanted with those).  Here is what I have been experimenting with:

Double Notching.jpg

 

I have discovered that the "notching" effect only occurs at the last opportunity, which is not a great contribution to the Body of Knowledge, but I cannot fathom the functions of the checkboxes 1 and 2.  In THIS exercise, checkbox 1 does nothing at any time! 

 

I cannot interpret the icons, I have no idea what these checkboxes are supposed to do.  Can you point me at some documentation which will clarify the issue for me?

 

Another curiosity I have is that, since the revolution on the right (the 'double dipper') is selected as a unit, why does the surface that makes select as individual units?  In this example I clicked on the last curve of the handle.

 

Thanks

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