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SKETCH DRIVEN LOCATIONS OF PARTS

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Message 1 of 13
RDG3PO
1035 Views, 12 Replies

SKETCH DRIVEN LOCATIONS OF PARTS

Former Solidworks user here turned Inventor user. I'm constantly running into roadblocks where I knew how to do something that Inventor just will not do. One of these is sketch driven locations of parts in an assembly. 

 

I'm tasked with locating a number of widgets in a case while taking up the least foortprint while affording the best amount of space between each widget. Formerly in Solidworks, I would contrain the planes of the widgets to a sketch and drag the sketch to adjust the size of my footprint.

 

Not surprisingly, this is a feature that's not intuitively available in Inventor. What would be the Inventor way of approcing this task? Make me love Inventor.  Thanks!

 

INVENTOR 2014 STANDARD
IOSX and PARALLELS
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12 REPLIES 12
Message 2 of 13
jeanchile
in reply to: RDG3PO

You can do the same thing in inventor you just need to constrain the items to the sketch entities (e.g. mate the cylinders of the parts to the center lines in your sketch).

We do this all the time using a part that contains the "skeleton" sketch placed inside the assembly then use constraints to lock everything to the sketch. I'm on my phone or I would post more info.

Good luck.
Inventor Professional
Message 3 of 13
RDG3PO
in reply to: jeanchile

Hey jeanchile, thanks for responding so quickly!

 

Maybe I'm blind, but when I choose the constraint option, I can select the features on the part no problem, but I'm not able to select the sketch entities. Is there some check box somewhere that allows you to select the sketch features? I've already tried changing the selection method from "Select Component" to "Select Sketch".

INVENTOR 2014 STANDARD
IOSX and PARALLELS
Message 4 of 13
jeanchile
in reply to: RDG3PO

Is your sketch an assembly sketch or a separate part "placed" into the assembly? We do this all the time with cylindrical objects and a sketch skeleton but I'll have to look into it further. I'm not at the office for the next two weeks and I'm having a new laptop built so I won't have access to IV until that's done and installed. Perhaps someone else can chime in while I get IV installed later today.
Inventor Professional
Message 5 of 13
RDG3PO
in reply to: jeanchile

I'm working on making a sketch in a separate part to place in the assembly. I'll letcha know how it goes.

 

EDIT:

This was in fact the case. I needed a sketch inside another part that was inserted into the assembly in order to constrain to the sketch. Seems really like a really backwards way of doing this, as I now have another layer of procedure to work my way through, and another part file sitting in a folder. 

 

Can anyone offer an explaination as to why this is necessary?

INVENTOR 2014 STANDARD
IOSX and PARALLELS
Message 6 of 13
jeanchile
in reply to: RDG3PO

While I'm certainly not qualified to speak intelligently about why the sketch needs to be in a part file I can offer my thoughts. In Inventor the assembly sketching tools are utilized primarily for creating assembly level feature like certain holes, machining features, etc. Using them for other things is permitted but usually not the best workflow.

 

Now that you have an effective "work-around" to accomplish the task at hand, it's at this point that I am going to ask a few further questions in hopes of determining a better method to achieve what you are after. Hopefully the really smart gurus like Curtis, JD, blair, et al will chime in here as well.

 

1.) What version of IV are you using (year and model)? YOu should consider putting this into each post so others can determine the proper help.

2.) Do you do this kind of case design often or is this a once in a lifetime kind of thing?

3.) Have you done a search for "case design" or "shipping container" or something like that here on the forum?

 

I'm guessing that using derived parts, multi-body parts, or another method is going to be the better choice for you if you do this often.

Inventor Professional
Message 7 of 13
RDG3PO
in reply to: jeanchile

I'm using 2014 Inventor Standard

 

We do these cases and others similar quite often, previously in a 2D cad system. I'm looking for the best possible work flow to do this, and so far the process isn't matching up with what I'd be used to doing in Solidworks.

 

I've looked in to using derived parts via "Make Components" but that starts to get buggy when I add or subtract layers from the parent part. End result is that I need the foam layers to output as a sheet metal file so that it can be sent to our CNC machine. In addition, I'm trying to set up our drawings so that as much as possible is done beforehand. 

 

I'll do some perusing on the forums today regarding case and container design. But anything one might have to point in the right direction would be really appreciated. 

INVENTOR 2014 STANDARD
IOSX and PARALLELS
Message 8 of 13
PaulMunford
in reply to: RDG3PO

You're going about this the right way. You may find it easier to include a number of user defined UCS's in your layout part. If you also have a UCS defined at the insert point of your parts out becomes very quick tip 'snap' them

 


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Message 9 of 13
PaulMunford
in reply to: PaulMunford

Sorry - my phone cut off...

...'Snap' them together using constraint sets...

 


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Message 10 of 13
riff62
in reply to: RDG3PO

I have started working on a program in VB.net that creates an assembly  based on a list of parts, with each part having a point defines in the list. The program reads the list, picks the correct part, and places it in the assembly. The list defines the point in the part as XYZ, theta, etc.and uses the point to place it at that location..It isnt finished yet, as I want the program to read the list, look for a part in a library, and place it. If it doesnt find the part in the library, it creates it, and places that new part.

The program is being developed to create an assembled model of a particle accelerator...beam tubes, magnets, etc..When I have time to finish it, it could potentially be used to create any assembly as long as it can read the list of parts, and at least 1 model of each part exists in the library.

 

(Paul, I think you and I might have talked about this at AU this year..)

Message 11 of 13
RDG3PO
in reply to: PaulMunford

Hey Paul, Thanks for the reply. 

 

I'm gonna have to look into using UCS points. It might work with some of what we do, especially if the locations were patterned. But sometimes we're just trying to get parts to fit however we can best make it work. Attached is a pic of the first layout I did using Inventor. We have rules to follow regarding distances to edges, and between components, but often times they are broken because the fit take precedence. In this case we had 8 each of three different components going into a case, but it's not always that easy. 

 

Locating the parts via a sketch that's contained in a separate part in the assembly has proved to be a giant PITA in this instance. It would have been preferable if I could locate the parts "free hand", and then extrude the outline of the cutout (drawn in a sketch at the parts level) down through the foam. But with the limitations(?) I've found with Inventor, getting from point A to point B is a little more convoluted. 

 

Screen Shot 2013-12-31 at 8.09.17 AM.png

INVENTOR 2014 STANDARD
IOSX and PARALLELS
Message 12 of 13
PaulMunford
in reply to: RDG3PO

Yep,

 

In this case I think I would derive the componet into the foam core part as a boundary surface, move body it around and then use that to generate the cut in the foam core liner.

 

Does that make sense?

 


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Opinions are my own and may not reflect those of my company.
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Message 13 of 13
RDG3PO
in reply to: PaulMunford

Hey Paul, that does make sense. I haven't got a chance to test it out yet though, to see if it works with our workflow. I will update here when I'm able to run through it. 

INVENTOR 2014 STANDARD
IOSX and PARALLELS

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