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Solidworks Sequence Drawings Workflow

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Cast Iron
Joined
Jun 10, 2009
Location
CA
I'm looking to improve our workflow for sequence drawings on some of our more complex jobs. We currently create sequence drawings and strip out all unnecessary features/information for each sequence to focus on. This has always required a separate model and drawing for each sequence. Issue we have is any revision that is early in processing requires that change to be made to every sequence model after this.

What I would like to do is create a single model, modeling it in the same order that we manufacture in, and be able to create drawings of each sequence in the same order. That way one change/revision to the model fixes all drawings associated with it.

I'd prefer to not roll back the feature tree. While this would work, it would effect other drawings. I'd prefer to not have to open the model every time a drawing needs to be updated and hide/suppress features.

Perhaps Master Modeling may be the answer to this, creating drawings off each child model rather than the parent? :scratchchin:

Any advice on this would be greatly appreciated. Thanks!

Note: It looks like Insert Part might be the ticket, to keep everything linked to previous sequences, but still creates separate models for each sequence. Not the end of the world, and might actually be cleaner on the Drawing end of it.
 
Not sure if this will help or not but do you understand what configurations are? They're very helpful for creating different versions or variations of a single model or assembly. Different drawings can be create from the variations by simply naming the configuration and each drawing associated with the process (Turn-1, Mill-2, Grind-3, etc.)
 
There's even a way to show removed material as a dotted line in the drawings, perhaps in the "phantom view" option. I used to use it a lot for showing range of motion or alternate position in assembly drawings and that's also possible by using configurations. Haven't done that in years due to different contract assignments and different CAD software so I'm a bit fuzzy on creating it but it occurred to me that this might be of some use in showing operational sequence of referenced material removal for shop drawings. Sort of a "Before/After" image to help explain the sequence without adding clutter to the drawing by just adding a notation to the dotted/dashed (or whatever type line you choose) to explain "Remove This". The configuration manager is a bit clumsy at first, like all other things unfamiliar, but once becoming comfortable it can open an entirely new set of modeling/drawing options. Hope this helps, good luck.
 
Like AD mentioned, configs are the way to go.

BugRobotics- Do you think there's an advantage to using the "Master Modeling" approach over configurations? Configurations can get a bit messy/complicated if too many iterations are used. This can be especially true if/when modifying components in a model/assembly that's trying to reference a constrained feature no longer there. This can also happen if a sketch gets re-drawn. Simple matter to remedy in the constraint manager but the "domino effect" can get messy commensurate with complexity of the assembly. Seems best to use configurations in a large assembly AFTER the design is finalized and set or it can become like wrestling an octopus.

Anybody else is cordially invited to comment here. If I only listen to my own opinions I'll never learn anything else.
 
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BugRobotics- Do you think there's an advantage to using the "Master Modeling" approach over configurations?

I don't.

Master modeling is excellent for creating multi-body parts that share common geometry that can be later separated into different parts/assemblies. It is my default style of modeling when designing assemblies that interface with any other part/assembly geometry. I would not use a master modeling technique to create a single part to show machining operation steps.

More than anything else, the OP's needs require planning prior to starting the part modeling to correctly create configs that don't break. Using base geometry that never changes (origin and the three basic planes) as the foundation for all other sketches/planes is probably one of the more important ideas behind creating models that are robust.
 
I haven't tried it with assemblies, but the technique I use for weldments is to use the "selected components" feature when creating the drawing. It's relatively quick to set up, and it updates automatically when the part is modified.
 
I have to ask are you the ones creating the parts or are you using parts created by customers?

If you, there is a multitude of ways to model the part\s to get what you want for your drawings, Configurations are the best way to do this.

Using a master sketch, contour select, multiple bodies, combine tool and as you go add a config at each step, then if something need to be hidden don't suppress, add a feature to fill, lastly if you need rads and chamfers add them last.

I use configurations all the time in SW to machine using HSMWorks, most of the parts are designed by the students (don't get me started on that) where poor modeling and underdefined sketches rule the day.
Most have multiple sided machining and the need for soft jaws or fixtures to hold so I modify their parts by adding material back for my configs as not to blow up the models.

drawings are quite simple after you get the model working clicking thru the configs, you can start one drawing and then save as to new name then change the controlling view to the config needed and the other views will update.

I taught CAD 1 here at ASU and had my student do this in one of the lessons for a manufacturing mill process for a part.

again you'll have to develop your way, won't happen overnight but eventually it will just become the norm. best of luck.
 
As others have already mentioned, planning prior to part/assembly creation goes a long way in making manipulation/revision easier and less trouble. Sometimes the design only has a desired effect/motion/result and the early design phase is all concepts explored, only to abandoned later or has unforeseen changes. Planning and strategies can be wasted time in the design concept stage IMO if it can/will be abandoned 25 minutes later for a better idea. Manufacturing tollgates often don't provide ample time for design exploration when the meter is running. Once the design is more or less set, configs and "Save As" are what I most often use to present/communicate with the various departments but always like to hear from others, thanks to all that took time to reply.
 
There's even a way to show removed material as a dotted line in the drawings, perhaps in the "phantom view" option.

This would be a great feature. We've added sketches on occasion for this but something automated would be ideal.

Master modeling is excellent for creating multi-body parts that share common geometry that can be later separated into different parts/assemblies.

Using base geometry that never changes (origin and the three basic planes) as the foundation for all other sketches/planes is probably one of the more important ideas behind creating models that are robust.

Very rare are we doing any multi-body parts or assemblies that need to go out to the shop floor, so I don't think Master Modeling will be the way to go. Not for this anyways.

I try and tie everything to the origin and main planes. Occasional offset planes from there but the models are robust. I rarely have any issues with models not regenerating after updating. No real issues there.

I have to ask are you the ones creating the parts or are you using parts created by customers?

Everything we make is off our customer drawings. More often than not though, we will model the parts ourselves and create internal prints/sequence drawings/CAM.

Before I saw the responses to this thread last week, I started messing with Insert Part and it has actually worked out really well for what I need, but I am going to dive into Configurations today as well. I appreciate all the responses so far. Thank you!
 
Late to the party, but at the bottom of the pane is a related feature called "display states" - which I've seen used in a webinar for solidcam, but not actually used myself. But they have uses related to configurations. (And I'd never even noticed the feature before the webinar.)
 
Late to the party, but at the bottom of the pane is a related feature called "display states" - which I've seen used in a webinar for solidcam, but not actually used myself. But they have uses related to configurations. (And I'd never even noticed the feature before the webinar.)

Display states are used more in an assembly for hide/show, color, transparency where you are not suppressing components. I use them all the time with HSMWorks, drop the part into the assembly as many times as I have configurations in the part, say I've got 4 of the part in the assembly at different configurations, then I add fixtures, sketches for boundaries and anything else needed.

thats where display states rock, hide and show in each display and no need to go to the tree and try to find the part.
 








 
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