Drawing - Too complicated to understand? How to simplify drawings?

[jamie.siddons]

Hi, 

I work for a joinery company, creating manufacture drawings for bespoke units.

I'm constantly having the issue of over-complicated paper drawings, and was wondering if anyone else has this issue? 

See attached an example to illustrate. The unit is complicated and has many parts inside. This would be difficult for a joiner to build, as its not clear what line is attached to another line. 

I know you can set the distance in a 'section', but doing this removes all of the lines behind, which just looks confusing, as it no longer resembles what i have drawn. 

This has obviously never been an issue when drawing in AutoCAD, but i'm not sure what the best thing to do in Inventor is. 

So i was wondering if anyone else has came across this issue before, and if so, any advice?

Also, on a side note: If anyone knows how to put the materials on a layer, and colour the hatched layer, that would help with this issue too! 

Thanks!

Jamie

[jamie.siddons]

Hi, 

I work for a joinery company, creating manufacture drawings for bespoke units.

I'm constantly having the issue of over-complicated paper drawings, and was wondering if anyone else has this issue? 

See attached an example to illustrate. The unit is complicated and has many parts inside. This would be difficult for a joiner to build, as its not clear what line is attached to another line. 

I know you can set the distance in a 'section', but doing this removes all of the lines behind, which just looks confusing, as it no longer resembles what i have drawn. 

This has obviously never been an issue when drawing in AutoCAD, but i'm not sure what the best thing to do in Inventor is. 

So i was wondering if anyone else has came across this issue before, and if so, any advice?

Also, on a side note: If anyone knows how to put the materials on a layer, and colour the hatched layer, that would help with this issue too! 

Thanks!

Jamie

[Jonka45]

Hi Jamie,

Not really sure what I am looking at here so I am making a best guess! We produce drawings of large assemblies (full vehicles) and have no issues with inventor. From moving from AutoCAD many years ago we did need a mind set change and needed to think about the structure a bit more. Is the whole unit 1 part, or does it have sub assemblies? Will the joiner make part A first then fix it to part B after to make an assembly (part C)? if so, can you draw the part A and the part B separately and then create a drawing of part C which shows how to combine part A and part B?

if you cant/don't want to split it down into sub assemblies then you could use level of detail and view reps. 

If you have created this drawing from an assembly then one way of simplifying that we use is to utilise view reps or level of detail. We use these to remove the bits inside/outside you don't need to reference so they don't show up in that particular view. This leaves only the bits you wish to see in the view and makes it "less messy".  If you are using multi bodies then you can turn individual bodies off when creating a drawing but its a messy way of doing it. You would be best converting it into an assembly and using view reps and level of detail.

If this information isn't of any help I would expand on your original question as you may get a few interpretations of the question posed.

Cheers

[Jonka45]

Hi Jamie,

Not really sure what I am looking at here so I am making a best guess! We produce drawings of large assemblies (full vehicles) and have no issues with inventor. From moving from AutoCAD many years ago we did need a mind set change and needed to think about the structure a bit more. Is the whole unit 1 part, or does it have sub assemblies? Will the joiner make part A first then fix it to part B after to make an assembly (part C)? if so, can you draw the part A and the part B separately and then create a drawing of part C which shows how to combine part A and part B?

if you cant/don't want to split it down into sub assemblies then you could use level of detail and view reps. 

If you have created this drawing from an assembly then one way of simplifying that we use is to utilise view reps or level of detail. We use these to remove the bits inside/outside you don't need to reference so they don't show up in that particular view. This leaves only the bits you wish to see in the view and makes it "less messy".  If you are using multi bodies then you can turn individual bodies off when creating a drawing but its a messy way of doing it. You would be best converting it into an assembly and using view reps and level of detail.

If this information isn't of any help I would expand on your original question as you may get a few interpretations of the question posed.

Cheers

[swalton]

We do product design for our customers.  Projects range from consumer electronics to rail cars.  We have to adapt our drawing style to match our customers' expectations.

---

@jamie.siddons wrote:

This has obviously never been an issue when drawing in AutoCAD, but i'm not sure what the best thing to do in Inventor is. 

Also, on a side note: If anyone knows how to put the materials on a layer, and colour the hatched layer, that would help with this issue too! 

Thanks!

Jamie

What is different from your AutoCAD drawing style to your Inventor drawing style?  What makes the Inventor drawings hard to read?  

Have you tried shading the views?  You can link the view to a Design View rep defined in the ipt/iam.  I tend to have a multi-color design rep active for design/modeling, then create a "painted" view to show the finish color of the components.  I'll show an iso-view of the complete assembly/part with the "painted" view active, then use the multi-color rep on the fabrication views. 

There have been a few requests for iLogic code that would place each component on a separate drawing layer.  Search the forum. 

I tend to recommend not using layers with Inventor drawings because most (all except linetype and line color?) of the AutoCAD uses of layers can be controlled by design view reps in the part/assembly file.  

Very Basic General Guidelines:

1. Detail each ipt file in a separate idw file. (or on different sheets of a multi-sheet idw if you must)
   1. These details show how to build that specific part.
2. Assembly prints show how the parts are joined to build the final object.  Think Lego building instructions.
   1. Add Exploded views and Cross Section views to show key details.
   2. Don't forget Detail Views.  
   3. Create Design View Reps (NOT Level-of-Detail Reps) to show different assembly steps and stages.
      1. LOD are a memory management tool.  Other uses are possible, just like I can use a screwdriver as a hammer.
      2. View Reps can be used to filter Parts Lists on drawings.  
   4. Shaded views can aid understanding.
   5. Written assembly steps or instructions on the drawing sheets
3. Provide the Customer a 3d copy of the assembly and a viewer.
   1. DWF, 3d PDF, STP, eDrawings are all options.
4. When you are modeling up the components, think about how the shop floor will manufacture the parts or assemble the components.
   1. Use this information when planning your drawing views.  Make sure the views communicate the critical information about how you expect the shop to fabricate the design.

[swalton]

We do product design for our customers.  Projects range from consumer electronics to rail cars.  We have to adapt our drawing style to match our customers' expectations.

---

@jamie.siddons wrote:

This has obviously never been an issue when drawing in AutoCAD, but i'm not sure what the best thing to do in Inventor is. 

Also, on a side note: If anyone knows how to put the materials on a layer, and colour the hatched layer, that would help with this issue too! 

Thanks!

Jamie

What is different from your AutoCAD drawing style to your Inventor drawing style?  What makes the Inventor drawings hard to read?  

Have you tried shading the views?  You can link the view to a Design View rep defined in the ipt/iam.  I tend to have a multi-color design rep active for design/modeling, then create a "painted" view to show the finish color of the components.  I'll show an iso-view of the complete assembly/part with the "painted" view active, then use the multi-color rep on the fabrication views. 

There have been a few requests for iLogic code that would place each component on a separate drawing layer.  Search the forum. 

I tend to recommend not using layers with Inventor drawings because most (all except linetype and line color?) of the AutoCAD uses of layers can be controlled by design view reps in the part/assembly file.  

Very Basic General Guidelines:

1. Detail each ipt file in a separate idw file. (or on different sheets of a multi-sheet idw if you must)
   1. These details show how to build that specific part.
2. Assembly prints show how the parts are joined to build the final object.  Think Lego building instructions.
   1. Add Exploded views and Cross Section views to show key details.
   2. Don't forget Detail Views.  
   3. Create Design View Reps (NOT Level-of-Detail Reps) to show different assembly steps and stages.
      1. LOD are a memory management tool.  Other uses are possible, just like I can use a screwdriver as a hammer.
      2. View Reps can be used to filter Parts Lists on drawings.  
   4. Shaded views can aid understanding.
   5. Written assembly steps or instructions on the drawing sheets
3. Provide the Customer a 3d copy of the assembly and a viewer.
   1. DWF, 3d PDF, STP, eDrawings are all options.
4. When you are modeling up the components, think about how the shop floor will manufacture the parts or assemble the components.
   1. Use this information when planning your drawing views.  Make sure the views communicate the critical information about how you expect the shop to fabricate the design.

[Jonka45 · Accepted solution]

https://cadsetterout.com/inventor-tutorials/how-when-use-autodesk-inventor-level-of-detail-represent...

Level of detail is a useful tool. It has limitations but don’t dismiss it. I agree if you listen to formal training then view rep is the way to go and is the way we mostly work but the ability to work and “draw” with more memory is useful with large assemblies or lower powered workstations. Drawings have got much better recently but large assemblies still take an age to render. If it wasn’t supposed to be used then it wouldn’t be selectable in the drawing.....now where is that screwdriver I have a nail to put in...

[Jonka45 · Accepted solution]

https://cadsetterout.com/inventor-tutorials/how-when-use-autodesk-inventor-level-of-detail-represent...

Level of detail is a useful tool. It has limitations but don’t dismiss it. I agree if you listen to formal training then view rep is the way to go and is the way we mostly work but the ability to work and “draw” with more memory is useful with large assemblies or lower powered workstations. Drawings have got much better recently but large assemblies still take an age to render. If it wasn’t supposed to be used then it wouldn’t be selectable in the drawing.....now where is that screwdriver I have a nail to put in...

[swalton]

---

@Jonka45 wrote:

https://cadsetterout.com/inventor-tutorials/how-when-use-autodesk-inventor-level-of-detail-represent...

Level of detail is a useful tool. It has limitations but don’t dismiss it. I agree if you listen to formal training then view rep is the way to go and is the way we mostly work but the ability to work and “draw” with more memory is useful with large assemblies or lower powered workstations. Drawings have got much better recently but large assemblies still take an age to render. If it wasn’t supposed to be used then it wouldn’t be selectable in the drawing.....now where is that screwdriver I have a nail to put in...

---

I agree.  LODs are good for memory management and improving large assembly performance. 

I'll argue a bit about using them in drawings, especially if I have to show a Parts List, or otherwise show 2 or more different LODs at once.  As your link discuses, each LOD shown in a drawing (including the Master LOD necessary for a Parts List) is an additional load of portions of the base assembly into system RAM.  

Opening the iam file at one LOD and the drawing at a different LOD can trigger some save warning messages too.

I see lots of folks try to use them as configuration management or view control tools.  I try to discourage those workflows.

[swalton]

---

@Jonka45 wrote:

https://cadsetterout.com/inventor-tutorials/how-when-use-autodesk-inventor-level-of-detail-represent...

Level of detail is a useful tool. It has limitations but don’t dismiss it. I agree if you listen to formal training then view rep is the way to go and is the way we mostly work but the ability to work and “draw” with more memory is useful with large assemblies or lower powered workstations. Drawings have got much better recently but large assemblies still take an age to render. If it wasn’t supposed to be used then it wouldn’t be selectable in the drawing.....now where is that screwdriver I have a nail to put in...

---

I agree.  LODs are good for memory management and improving large assembly performance. 

I'll argue a bit about using them in drawings, especially if I have to show a Parts List, or otherwise show 2 or more different LODs at once.  As your link discuses, each LOD shown in a drawing (including the Master LOD necessary for a Parts List) is an additional load of portions of the base assembly into system RAM.  

Opening the iam file at one LOD and the drawing at a different LOD can trigger some save warning messages too.

I see lots of folks try to use them as configuration management or view control tools.  I try to discourage those workflows.

[johnsonshiue]

Hi Guys,

I am wondering if Slice View can help. Also, using Design View Representation is better approach than Level of Detail.

Many thanks!

[johnsonshiue]

Hi Guys,

I am wondering if Slice View can help. Also, using Design View Representation is better approach than Level of Detail.

Many thanks!

[Jonka45]

https://blogs.autodesk.com/inventor/2016/08/23/represent-with-level-of-details-or-view-reps/

Jamie,

just a bit more on what we have been discussing. This is the way I was trained to deal with view reps. I still use Level of details in some instances. Though and I agree that there can be issues in doing so especially when you have the drawing open in one LOD and try to change the model in another LOD it can get messy when saving or trying to save. 

Listen to Swalton and johnsonshiue they are offering the correct workflow.

Good luck 

[Jonka45]

https://blogs.autodesk.com/inventor/2016/08/23/represent-with-level-of-details-or-view-reps/

Jamie,

just a bit more on what we have been discussing. This is the way I was trained to deal with view reps. I still use Level of details in some instances. Though and I agree that there can be issues in doing so especially when you have the drawing open in one LOD and try to change the model in another LOD it can get messy when saving or trying to save. 

Listen to Swalton and johnsonshiue they are offering the correct workflow.

Good luck 

[IgorMir]

Hi Jamie,

I will start with offering you to have a look at the Standard Editor. Just as it is shown in the image attached. In the editor you should be able to specify the colours for the drawing's entities the way you like it.

Secondly - I don't see what's the fuss is all about? The picture you have posted is a clip from the assembly drawing. The clip, as it stands - is meaningless. But the assembly drawing is just an instruction - how to assemble the product, not how to build it. it should contain the links (in a form of the Part List),  to the components of the assembly. And those components are represented by the detail drawings. Once you have a proper system of documenting your design in place - your drawings will be a breeze to read. And a good place to start from will be the National Drafting Standard.

Cheers,

Igor.

[IgorMir]

Hi Jamie,

I will start with offering you to have a look at the Standard Editor. Just as it is shown in the image attached. In the editor you should be able to specify the colours for the drawing's entities the way you like it.

Secondly - I don't see what's the fuss is all about? The picture you have posted is a clip from the assembly drawing. The clip, as it stands - is meaningless. But the assembly drawing is just an instruction - how to assemble the product, not how to build it. it should contain the links (in a form of the Part List),  to the components of the assembly. And those components are represented by the detail drawings. Once you have a proper system of documenting your design in place - your drawings will be a breeze to read. And a good place to start from will be the National Drafting Standard.

Cheers,

Igor.

[jamie.siddons]

Thank you for your replies.

I have been using Inventor for a while now, and I have admittedly never came across the Level of Detail and Drawing Reps options. I watched the the video that was linked, and it's solved a huge part of the problem! The drawing I attached is a circular unit, and with so many hidden lines all showing at once, it is difficult to understand. View reps will definitely help solve those issues!

---

I've managed to use Styles to hatch individual parts based on its material value, but is this possible with colour too? It would be good if I could use colour in my drawings to show varying materials? I'd rather not use shading, as it uses a lot of ink when printing. Has anybody managed to do this? I assume it's possible by assigning materials to layers?

Thanks!

[jamie.siddons]

Thank you for your replies.

I have been using Inventor for a while now, and I have admittedly never came across the Level of Detail and Drawing Reps options. I watched the the video that was linked, and it's solved a huge part of the problem! The drawing I attached is a circular unit, and with so many hidden lines all showing at once, it is difficult to understand. View reps will definitely help solve those issues!

---

I've managed to use Styles to hatch individual parts based on its material value, but is this possible with colour too? It would be good if I could use colour in my drawings to show varying materials? I'd rather not use shading, as it uses a lot of ink when printing. Has anybody managed to do this? I assume it's possible by assigning materials to layers?

Thanks!