increasing an extrude without stretching the sketch

[Anonymous]

Hi all,

Done a search and haven't found answers to this curiosity. I need to enlarge an object in the direction the extrude was formed. If I increase the extrude, it stretches the existing sketch unhelpfully. I'd like to increase the amount of material to adjust my sketch into.

Thanks,

OLC

[JDMather]

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@Anonymous wrote:

... If I increase the extrude, it stretches the existing sketch unhelpfully.

OLC

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Something sounds very very wrong with this.

Can you attach the actual *.ipt file here?

[mcgyvr]

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@Anonymous wrote:

Hi all,

Done a search and haven't found answers to this curiosity. I need to enlarge an object in the direction the extrude was formed. If I increase the extrude, it stretches the existing sketch unhelpfully. I'd like to increase the amount of material to adjust my sketch into.

Thanks,

OLC

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No it won't unless maybe you are editing a parameter to adjust the extrusion length and that parameter was used in the sketch also

As stated.. Please post your ipt file to investigate.

[Anonymous]

A zip folder containing most of the files is attached. Some bodies are in different folders but aren't part of the problem. I've attached two pictures also showing the problem. In assembly, I select 'chainstay' and edit. I need to alter the first extrusion to give me more width to the chainstay but, as you can see in the second picture, the extrusion stretches the existing sketch which really burns my marshmallow. What do you reckon?

[JDMather]

Are you OK with following step-by-step instructions to remodel from scratch and learn to do this all correctly (there are a significant number of issues in the technique).

Warning:  I have only had one person who answered yes to this question follow through on following my instructions.

[Anonymous]

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@Anonymous wrote:

Are you OK with following step-by-step instructions to remodel from scratch and learn to do this all correctly (there are a significant number of issues in the technique).

Warning:  I have only had one person who answered yes to this question follow through on following my instructions.

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Yeah, some tuition would be appreciated. I've been signed off work for three weeks and the assembly you've seen represents everything I've achieved in that time but I've obviously got some bad habits that need correcting. And I'm keen to get this project assembled accurately because I intend on 3D printing this project and actualising it. I've got exactly a week before I'm back to work, in which time I hope to have the virtual projection completed.

Cheers JDM

[Anonymous]

Bump,

I'm hoping that JDMather will have time to write up some advice, but if not, I'm not easily able to resolve the extrude/stretch problem to finish the tollerances on the design. Any advice greatly appreciated.

Cheers

[JDMather]

Start a new part file.

Create the sketch as shown and then attach your *.ipt file here.

Collet 47 - Sketch1.png

[Anonymous]

Cheers,

First attempt attached. First question, I don't know how you dimensioned the diameters - I have dimensioned to the centre point only.

Aaron

[blair]

If you notice in JD's post, he has used the "Centerline" in his sketch. This then forces Inventor to create the dimensions as shown in JD's post. You only have a work point that you are dimensioning to.

Delete your dimension, construct a vertical Center Line (need to change the line type t Center) and then dimension from your object to the Center Line and you will get the correct dimensions.

[JDMather]

This is a screen capture image of your sketch.

Note that one of your lines has not changed to a darker color (fully defined).

Note that in the lower right corner of the screen Inventor indicates that the sketch is not fully constrained.  (Geometry Constraints can be (and usually should be) used in place of dimensions to fully define the sketch.)

Diametral Dimensions.png 

Get experienced with using Construction Lines and Centerlines.

You can toggle to these linetypes by right clicking on a normal line.

To get a diametral dimension you must have a Centerline type.

These are keys that will make you design life much easier in the future.

[Anonymous]

Ok, I'm there. I hadn't paid enough attention to all of the construction lines in your original post which made dimensioning in the same way you had impossible. But it's all in now. Things learnt already 🙂

[JDMather]

Now add a 2-Point Center Rectangle as show to the sketch.

2 Point Center Rectangle.png

[Anonymous]

Double post

[Anonymous]

I'm there.

[JDMather]

Revolve the outer portion of the sketch.

Then right click on the sketch and turn on Visibility.

Extrude-Cut through all with the rectangle.

Assign material so that the part will have the correct Mass.

Save As Collet 47 

and Save As Copy Collet 47b.

Next we will edit sketch dimensions to correct sizes.

Revolve Then Extude - Cut.png 

Assign Material.png

[Anonymous]

Yup, all there.

[JDMather]

I think that you didn't realize what part I was going to start with - I always start with something simple and work towards the more complex.

In your assembly these were the collets.

Note that you can simple double click on the dimensions to edit to correct sizes and everything will update without breaking because we fully defined the geometry.

You should now be able to properly model the rest of the easy cylindrical parts.

Now let me look at one of the more complex parts.

Hmmm, I see issues with the Seatstay.....

[Anonymous]

I assumed the shape was going to be the extrusion for the hollow which accepts the collet. But this process has got me thinking about which is the important part of a design to start with, I did the chainstay first and then built the hollow (as you'll have seen). I can see the benefit of ensuring the part is dimensioned correctly, especially when there are similar parts or a likelihood of adjusting sizes...

[Anonymous · Accepted solution]

I've re-looked at the sketch of the chainstays and I think there were references to projected edges. So when I extruded the shape, the referenced edges moved and warped the sketch. I've redefined the sketch and it now extrudes in the correct way.

Cheers