Automotive industry 3D Design policy in SolidWorks 2

[MateuszM]

Hello,

I have a question about design policy in automotive industry when it comes to the 3D Design.

I work as a CAD Engineer in the company which asprates to be automotive - it means we are transforming from small garage manufacturer to something bigger and much more organised.

We use SolidWorks to create all the 3D data and it's no problem, but recently we have employed new Design Director who has some experience with automotive industry (as far as I know Ford, VW), but he is not a mechanical engineer, but designer and he works in Rhino.

To the point now - he claims that it is common in automotive industry to base all parts from complete assembly origin point (VW takes it in the middle of front wheels rotation axis for example) and now I should model all new parts not starting from point 0,0,0 of new part file, but for example - from -1200,500,350 and then it's already on it's place when added to the assembly and mated with the origin planes.

For me it's against how the mates in SW work, but maybe I'm the one who is wrong?

I think it's OK to have common origin point of whole vehicle assembly, but relaying on the plane mates instead of standard SW mates makes no sense for me.

What is your opinion about it?

Thank you in advance.
Best Regards.
Mateusz

 

[GregLocock]

Won't work. For example, if you draw a wheelbolt (silly but obvious example) it could be in any of 5 locations, in the local coordinate system, and then if a different model (say the GT) is at a different ride height at design then it could be somewhere else.

However the answer, as always, is to pick up the awfully heavy phone and ask your customer.

Having said that shifting the whole thing and rotating it is not a big job, so you can do it his way.



Cheers

Greg Locock


New here? Try reading these, they might help FAQ731-376

http://eng-tips.com/market.cfm?

 

[MateuszM]

Thank you for your opinion Greg,

Unfortunately I can't ask customer as we do it for our internal purposes, there are two CAD engineers in our company (SolidWorks) and now one design director (Rhino). Sometimes we outsource our production to another companies so the idea for this was to avoid missalignment when transferring to another CAD systems.

I'm closer to your opinion, but here is an another answer I've got from another board:

"...that makes airplanes works from a co-ordinate grid central point that may be a long way off, much like you have described. He referred to that point as "airplane zero" and all parts had to reference that point in creation and assembly. It may seem odd but there is a logic to it when the assembly is huge and locating parts can be easier when simply looking for a co-ordinate location in that assembly rather than panning over a sea of parts that may be similar. How could you describe a component location to a co-worker in another country if not for a global co-ordinate system? Constraints change with revisions, assemblies can explode, and non-native program files may not import as expected. One thing that can remain constant is "airplane zero". It's likely a bit difficult to work with but I can see a certain logic to this."

and:

"For complex assemblies with large number of components, plane mates are better since, if you make changes to the mating model geometry (edge, surface, point or line) errors are not generated into the assembly mates (as usually happens in geometry mating) .

Also starting a new 3D model by taking co-ordinates relative to the main assembly origin is basically a time saving technique. So that when you are assembling, you don't have to think much, just mate the planes and you good to go. Hence, this technique along with plane mating are meant to save time and improve accuracy of assembling.

The down side is that before commencing modelling, you have to be very sure of the co-ordinates and the orientation of the new model as you will not be able to play around with mating axes during assembly."

So there are ups and downs as usual. Maybe the mixed approach would be suitable? As some parts have their specific positions and are always on the same place in every model so can be mated by planes and those which are in various positions could be mated using standard mates.

All in all I'm the employee here so I'll have to adapt.

Thank you.

 

[GregLocock]

That make sit easier. You've been told what to do. If it is wrong you'll find out. I doubt VW will be using SW, I know Ford don't, so nobody is going to be relying on your mates working.

Cheers

Greg Locock


New here? Try reading these, they might help FAQ731-376

http://eng-tips.com/market.cfm?

 

[SwinnyGG]

No major automotive manufacturer uses Solidworks as their base CAD format. Even if they did, you NEVER want to give full models to customers, unless they have paid you for full engineering rights AND you have an AIR TIGHT non-disclosure agreement with said customer.

That's a contract issue which is most likely out of your scope, but it is good engineering practice to assume that any transfers of 3D data, unless explicitly stated otherwise, should be handled by conversion to a universal interchange format (IGS or, preferably, STEP AP 214) with all model tree data stripped out, and only required external surfaces/bodies available for viewing.

Transferring full models means larger files that are more difficult to manage, not to mention the fact that you are sending your company's intellectual property out into the world where anyone can access it.

Secondly, in order to base all design work off of a universal coordinate system, you would have to know to high precision the location and relative orientation to the vehicle coordinate system of every part you model. This is an impossible ask.

Adding a part to a model and mating it correctly in its proper location is part of the design process. If your assembly build-out process consists of adding parts to the model and mating to the global csys only, you are missing a huge portion of the checks that need to happen during assembly.

You won't catch part interferences, you'll miss parts that don't fit, and if you have multiple locations for the same component, your process doesn't accommodate that.

In short, modeling every component from an assumed global CSYS is terrible design practice, and it causes many more problems than it solves.

I've had this request from customers before, and in every case I've told them to pound sand. Your new director sounds either inexperienced or clueless about the design of large assemblies which contain hundreds or thousands of parts. Maybe both.

 

[RobWard]

We do work for automotive and aerospace companies and a most models we get from them come with an common assembly origin point. Sometimes this is 10's of meters outside a component.
It was explained to us just why (pretty much the reasons given above), but its a right royal PITA for us when working with their models.
Solidworks doesn't seem particularly good at allowing you to change the reference frame simply, and when you'r dealing with organic shapes with no natural origin or axes of their own it can be a real challenge to reorient them to something sensible.
That said, we send them our models back with the origin in the part and they have yet to complain, or even comment. Maybe they're better at this than us. (They are DEFINITELY better than us!)
They all are able to provide us with Solidworks models (not just .stp files), though I believe they actually use Catia primarily themselves. Perhaps that's a courtesy that they extend to their supply chains just for practical reasons.

"I love deadlines. I love the whooshing noise they make as they go past." Douglas Adams

 

[CWB1]

Your new director is correct and not just about the automotive industry. Standard modeling practice everywhere is to store files based off a standard universal coordinate system. When you're designing a part or assembly, you work parametrically using whatever mates/references are available in the given software package to ensure a good relationship between the new parts and surrounding existing parts. Once design is done however, everything within your new part/assembly needs to be referenced back to itself to ensure that when others change their parts yours do not change fit, form, or function due to existing mates/references. Your new parts can have their local UCS referenced back to a master company/vehicle/product UCS, typically the local and master UCS are simply made coincident to one another, however in the case of supplier parts its common simply to define the distance and orientation of planes vs the UCS bc suppliers typically don't have access to the vehicle/product model. In essence, that is what happens automatically when multiple instances of the same part are assembled.

Not sure what your company's ultimate goal is, however something else to be aware of are the limitations of Solidworks. Given its very limited capability for handling complex assemblies and surfacing you may want to begin transitioning to a proper engineering modeler. Not to knock it, but Solidworks is a pretty basic modeler intended for use on the shop floor by folks with very limited training and needs, not really something commonly used in engineering design. The two biggies in most mechanical design today is Dassault's CATIA and PTC's Creo.

 

[MateuszM]

Thank you for all your answers, now this topic is much more clear for me.
We manufacture vehicles but as I see we are far from automotive yet - I'm affraid the combination of SolidWorks and Rhino is the best combination I could have for now and it's much more than I've had when I've started work here (a couple of dxf files for laser cutting, and the whole closet of 2D documentation drawn by hand).
Best Regards.
Mateusz

 

[KiwiME]

Interesting post. I used this UCS concept initially way back in the late '80s with AutoCAD 10 in 3D, for low-volume electrical cabinets mostly. After drawing a part in the 'assembly' from thick polylines and circles I had a Lisp function to create a block out of the selected entities and re-insert that back at 0,0,0 having only needed to supply a name and the colour number. This was primarily to lock-in the relationship between all entities comprising that part to avoid the risk of other designers accidentally moving them when working on the same assembly. If anything got moved it was the entire part, easier to spot.

In SW I did a similar thing for the practical reasons stated by CWB1. SW mates based on features found in other parts can easily be damaged or inadvertently moved and so each part is designed around planes offset from the default UCS, the latter which is common to that in the assembly. Once a project is completed it just makes everything more durable.

 

[BUGGAR]

Interesting, KiwiME.
I think you ideas would work well with my projects where I have to "collect" parts from design drawings and turn them into dxf files ready for the water jet.