Hatch lines

[Anonymous]

I've got a small problem. For my engineering class i have to turn in a set of drawings of an assembly. When a part is sectioned we are only allowed to use 45° and 135° hatch lines and if the part is show in a other section it has the be the same style (dahh) . Right now I have to edit every view by myself. Is there a faster way where Inventor does that automatically allocating a unique style to every part so I don't have to spend so much time on that?

Thank's in advance

Nils

[Jose_Merino]

In your Style Editor go to Hatch, and there you can make the hatch that you want, and use it every time.

[Cadmanto]

In conjunction with @Jose_Merino see the attached link.

https://knowledge.autodesk.com/support/inventor-products/getting-started/caas/CloudHelp/cloudhelp/20...

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2018

[Anonymous]

I already went into the Style Editor and under Standard I changed the available Section Hatch Angle to 0° and 90°. But my problem is still that Inventor uses for two different parts the same scale and angle or when the same part is visible in a different sectioned view it has a different angle and scale. Is there a way to have it all the same over the entire drawing?

[Anonymous]

As far as I understood that tutorial you can add hatch styles to certain areas. But I already got the hatch style I want with ANSI 31. The only problem like i stated above is the scale.

[johnsonshiue]

Hi Guys,

I think this could be related to the preset hatch variation angle values, if I understood the request correctly. There is an easy-to-miss workflow. Go to Manage -> Styles Editor -> select the active standard -> General -> Preset Values -> select "Section Hatch Angle." There you can define the various values to differ hatches in the same style.

Many thanks!

[Anonymous]

Yes that archives the first part in the lines being only 45° and 135° angle. But can I tell Inventor now that for every part of an assembly each should have a unique combination of Angle and Scale which will be the same throughout the entire drawing. Right now I have to check every view for that. Maybe the screenshot will clarify. Part 1, 7 and 11 have the same angle and scale. And in section D-D those values change.

[johnsonshiue]

Hi! I am sorry I may have misunderstood your request. The way the angular variation works in Hatch is that different components with the same material style would have the same hatch but in different angles. Based on the image you are showing, the function does not seem to work. Something is wrong. Please share an example here so we can look into further.

Many thanks!

[Anonymous]

I'm sorry for replying so late, had lot's of stuff to do. What would you need for that? Just the .idw or something else?

[johnsonshiue]

Hi! I need the idw/dwg file and also the component files (ipt and iam) referenced by the drawing.

Many thanks!

[Anonymous]

This should be all the files you need. If you need anything else tell me.

Thanks

[johnsonshiue]

Hi! Many thanks for sharing the files! I think know what you are looking for. I guess you are not aware of a workflow called assigning hatch pattern to material. In the Drawing Styles Editor, you can assign specific hatch to each material. Then, the material specific hatch patterns will be shown. Please take a look at the following workflow. It should work for you.

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/screencast/Main/Details/...

Thanks again!

[Anonymous]

But that only keeps that style of hatch pattern to one material and you would still have to edit every part(because we are only allowed to use the ANSI 31 style as pattern). I guess what I'm really looking for is something like assign specific hatch to each material only for parts in my assembly so I could predetermine the angle and scale of each part. 

[johnsonshiue]

Hi! No, you don't need to edit every part or every drawing to make it work. First, you need to decide what hatch style you want for each material. Then set it up in Styles Editor -> Standard -> Material Hatch Pattern. Then save the style to Style Library. After that, there is a batch update tool shipped with Inventor to update all drawings with the updated style. The various hatched will be displayed in the drawing views.

Many thanks!

[Anonymous]

But as far as I understood the video it would only allow me to assign a style to every material. Is it possible to let it differentiate between 2 or more different parts of the same material? Like:

part 1 ANSI 31 45° and scale of 1

part 2 ANSI 31 45° and scale of 1,5 

and so on...

Or is that something i would have to assign manually.

Thanks for the time even though it might feel like talking to a brick wall:)

[johnsonshiue]

Hi! Unfortunately, such workflow is not allowed. Is this a special standard you are following? Why do you need the same material having different hatch scale? For detailing purpose?

Many thanks!

[Anonymous]

Well it's a pretty harsh interpretation of DIN ISO 128-50. Still thank you very much for your time even though you couldn't help with this.

Cheers