Drawing questions

[Jim-Nolan]

A few questions on drawings. I have created a drawing of an assembly from an animation. Part of the assembly is this angle component (s), originally a sweep along a path. In reality it was always going to be made from machined ends and some angle. Subsequently it was cut where it crosses three webs using the combine tool. This produced separate bodies for each piece. I converted the bodies to components so I could copy the ends into a new drawing for CNC manufacturing the ends.

I then created the animation from the whole assembly, inserting a table into the drawing, the balloon only points to the angle as one piece. Not three balloons  at two off each?
Secondly where I have mirrored, or copy>moved components the balloon points to one but the quantity in the table doesn't reflect the mirror or the copy move ?

[andrew.de.leon]

Hi @Jim-Nolan,

Sorry to hear you're having troubles with drawings. Without seeing your drawing, make sure all components except Angle (the assembly containing the individual components) is suppress before creating a parts list. This will force the parts list to change what it considers the top level assembly; it will use the Angle assembly as the top level instead of the selected storyboard and should balloon the 4 pieces. You should be able to add additional balloons if needed.

Tip, to suppress everything except the Angle assembly, right mouse click on the Angle assembly in the browser and select Suppress all except selected. You should be left with only the Angle assembly's components within the drawing.

If this doesn't work, please send me a screen shot of your drawing open in Fusion so I can see your browser and we'll go from there.

Cheers, Andrew

[Jim-Nolan]

Hello Andrew,

That advice didnt work for me. I have attached some snaps of the drawing the ballons were generated with the tree closed up. I also attach a snap with the angle expanded so you cna see how i arranged everything

Thanks 

Jim

[andrew.de.leon]

Hi Jim,

Thanks for sending through a few more images. I assumed the Angle assembly (item 4 in your parts list) was the only assembly you were trying to document but that doesn't appear to be the case. Unfortunately, our parts list is limited to top level components only. As a result, only the components directly below the Top Cover Assembly can be included in the parts list and balloons; the components within the Angle assembly cannot be included.

We are currently working removing this limitation and supporting an all-level parts list but we've only just started development on this so I can't say yet when it will be available. Once available, you'll get a parts list including the entire assembly structure. The components within your Angle assembly (item 4) would be shown as items 4.1, 4.2, 4.3 and 4.4. Does this sounds closer to what you're looking for?

To get the result you're looking for now, you'll need to modify your Top Cover Assembly and move the components within the Angle assembly up one level into the Top Cover Assembly. Then remove the empty Angle assembly. The parts list will then see all components and balloon them accordingly.

Cheers, Andrew

[Jim-Nolan]

Hey Andrew,

Thanks very much for the comprehensive reply. As a hobbyist this was the most complex drawing I had done. I normally just do one component to get into the manufacturing workspace to produce the CAM strategy and G code for my mill. The box assembly under the lid was what I needed this time, to produce a tab and slot assembly for laser cutting.  The assembly drawing was more of an intellectual exercise after watching one of Bad Tallis's videos. The 4.1 , 4.2 idea seem a good one though.

Would you care to comment on the second part of my question as to why the list does not reckognise the correct quantity's where I have mirrored a component or copy and moved it, item 5.6.7. 9 and 10 on the snap are examples of this. Is this also a software limitation ?

Thanks 

Jim

[andrew.de.leon · Accepted solution]

Hi @Jim-Nolan, 

Sure thing! Sorry I missed that part of your question.

No, this isn't a software limitation. Currently, the mirror command is designed to produce a true mirror of the component; where the mirrored part is side specific and therefore doesn't have the same geometry. However, there are cases like yours where the geometry is symmetrical and a mirror would work. Unfortunately though, mirroring still creates a new component rather than an instance. As a tip, you can tell the difference by looking at the component names in the model's browser. If all component names are followed by ":1", it's a good indication you have unique components rather than instances. Instances will have the same name followed by ":1", ":2", ":3", etc. This difference is critical when you then create a parts list in drawings. The parts list sees each component and itemises them accordingly. If multiple unique components exist; all components are followed by ":1", you'll get each component itemised separately with a quantity of 1. If multiple instances exist, you'll get each unique component itemised separately and a total quantity for instances of the same component. Hope that makes sense.

Copying and pasting (Ctrl+C and Ctrl+V) should have resulted in instances by default. Although there is an option to Paste New which does result in a new unique component rather than an instance. You'll see this by the new component's name changing to "Component(2):1", "Component(3):1", and so on for Paste New and "Component:2", "Component:3", and so on for Paste (Ctrl+V).

So how do you resolve this? I would suggest using either copy\paste (Ctrl+C and Ctrl+V) and then assembling using joints, or possibly using a pattern; either rectangular or circular (if a rotated 180 degree copy is needed). As an example, I've attached a crud examples of my work bench below. I've used circular and rectangular patterns to get around the same issue you have.

Hope this helps. Keep me posted on how you go with it.

Cheers, Andrew

[Jim-Nolan]

Hey Andrew,

Thanks so much for the comprehensive reply. I am not that sure I understand it fully especialy the bit about the mirror command being side specific, or that it may not be symmetrical or have the same geometry. To me a mirror is a mirror, but that is probably because I live in a far simpler world 🙂 

Thanks once again for your time this has helped a lot.

Jim

[andrew.de.leon]

Hi @Jim-Nolan,

No problems. And regarding the mirror, I probably didn’t explain it too well. Think of a pair of shoes where you have a left and a right, the mirror command allows you to design the left, then mirror to create the right. In your scenario, although a mirror can be used, the components are identical, so a copy and 180 degree rotate would be the better workflow. I hope this makes more sense.

Anyways, hope it helps and feel free to reach out if anything else comes up.

Cheers, Andrew