make layout or framework for cabinets

[nikhil]

hi can anyone help me about how to make the layout or framework for cabinets of p.c.b.( inside n outside both) its similar to the cabinets of our p.cs but the slimmer vesion.

pls help me out

[JD Mather]

I think I would use Autodesk Inventor with it's Sheet Metal tools. Can automatically generate flat patterns from your "as folded" design. Inventor also has plastic feature tools and Inventor Tooling can be used to automate the mold making process.

 

BTW - Need Help is not a very good thread title, everyone needs help. Doesn't help others search for solutions to their similar problems. Only takes a bit more time to think up a descriptive title.

[nikhil]

thank n my apologies for the thread title...im jst new around here,anyways thanks alot for replying for my query.

[Cad64]

The thread title has been renamed to something a bit more appropriate.

[nikhil]

thanks cad64...will be learning alot from u guys.

[nikhil]

hi JD,i am now using autodesk inventor 2008 for the sheet metal...but i am stuck on how tojoin the conners after attaching the flange...require ur help...i am attaching the pic of the file.

[JD Mather]

Zip and attach your file here.

[nikhil]

Zip and attach your file here.

 

sending the zip file....can u also tell me the steps to do it...

Part2.zip

[JD Mather]

First thing I notice is that your Sketch1 is not constrained. Read this document and fix Sketch1

 

http://home.pct.edu/~jmather/AU2006/MA13-3%20Mather.pdf

 

iProperties indicate that you are using v2008 and have not installed the Service Packs. You should install all SPs and Hot Fixes. You should indicate when you are not using the latest release of the software.

 

You should have used a Face rather than Extrude for the first feature.

 

I assume something like this is what you are after.

[nikhil]

ya thats what i was looking for...thanks alot for solving it.

i did try by using the face but may be i could'nt do it right...really thankful for the help as well as the pdf file...need to go home and have a look at it...thanks again

[JD Mather]

Let me show you how to simplify this part.

As much as possible you should use origin planes rather than part faces for sketches.

 

Create Sketch1 as shown. Notice the position of the Origin Center Point.

[JD Mather]

Exit Sketch1 and start Sketch2 on perpendicular Origin workplane.

Create the vertical line at the Origin Center Point as shown (note that your sketches change color when fully constrained).

 

(I turned off visibility of dimensions in Sketch 1 for clarity.)

[JD Mather]

Now go ahead and use the Face tool.

Then select the Contoured Flange tool and select the vertical line from Sketch2.

Then click all three of the 3 bottom edges of the Face, starting with the edge that actually attaches to the 6mm line.

 

Your screen will look a bit different than mine - if you were using a later release of inventor, not from the image that you could take care closing the corners at this time.

[JD Mather]

Because you have an earlier version of Inventor you will have to edit the Corner Seams as separate steps.

Start the command and click the two outer edges.

Set the desired gap (keep in mind that we cannot manufacture perfect parts - there will be a plus/minus tolerance associated with cutting the flat pattern).

Set the corner style (your dialog box might look slightly different than mine.

Experiment with every selection order and setting in this command until you understand everything it does.

[JD Mather]

I just realized that earlier I gave you some bad information.

You USUALLY should create any sketch you can on an origin workplane rather than on a part face.

Sheet metal parts are one time when you don't try to always adhere to that general rule.

For example - if you wanted a cut to wrap around a bend you need to create the sketch on the part face.

Since in this part your cuts do not wrap around the bend I would use the workplane. Be sure to dimension size and location of cuts in your sketch.

 

(you don't need to turn the workplane on to use it - you can select from browser when starting a new sketch, I simply turned it on for clarity. The reason you try to use work planes when possible is that when editing features you could cause a dependent sketch to go "sick". This can be avoided by using the origin geometry.)

[nikhil]

thanks JD it was really helpful.....thanks again

[nikhil]

hi JD...sry for troubling u again...." i have two similar parts for my assembly.so if i make one then can i copy n paste or do i have to make it as another component" i hope u got my question...

[JD Mather]

Save As new file name and edit the dimensions on the new file.

[nikhil]

alrite...let me try n see...thanks again

[JD Mather]

I forgot to mention another method.

If you have several parts that are identical except for a few features (like cuts, holes) do one part and then do Derived Components for the others. By this method if you need to make a change to all you make it in the original and all of the derived components update.

Another technique is iParts.....