Just looking for some helpfull advice 2

[Bellerophon]

I work for a company that makes steel doors and windows. Currently we do all of our drafting work with Autocad LT. when we start a new job, each door must be drawn from scratch/template to match the specific size and hardware requirements for the job. This way has worked well for us in the past but now that our workflow has increased we are starting to see more and more user errors in the drawing stage resulting in miscut parts ect. In order to resolve this we have recently purchased Solid Edge 16 and are hoping it will help steamline our process a bit.

Our ideal goal is this:

1) recieve a job consisting of door/window sizes, hands, glazing and hardware group details
2) input that data into an excel spreadsheet linked to Solid Edge
3) have solid edge recalculate door dimensions,hand and place the corresponding hardware on the door as called for by the hardware group number.
4) have solid edge print cutsheets and hardware list sheets to be issued to the shop floor for manufacturing.

All of this with as little user interaction as possible with Solid Edge. How attainable are our goals here?

and now for a few random questions:

1. In order to change the hand of a door (ie left hand reverse, right hand, left hand , left hand reverse; which way it opens.) am I going to have to create a template for each hand or is solid edge able to flip flop orientations of parts via a variable such as this?

2. Our Autocad drafter will continue to do things as we always have whilst I come up with an efficient means of implementing solid edge and eventually replacing autocad. I however have no engineering background though I'm quite handy at making and maniplating parts via solid edge after just completing the tutorials. I'm schuduled for the intro training classes and have purchased a book. Is there anything else I can do to help ease into this program?

3. should I spend my first few weeks just building up a basic parts compilation and then worry about assembly later on?

I'm sure I'll have many more questions. Thank you for taking the time to read and respond to this!

 

[PatCouture]

Hi Bellerophon

Welcome Aboard! First of all, even with the introductory class you won't be able to build your ultimate assembly with all the relations you want to put trough your model the week after.

From my standpoint, the best thing is to draw a prototype model and test solid edge by yourself. Be prepared to start over and over because you will discover many little details that solid edge does and you don't know about. Go with a very simple and easy door with let say 5 parts or less to simulate the handle, the lock etc. then make change to the door and see for yourself what happens.

The class, the book and this site is a very good way to start but it's very though to have a step by step procedure to do exactly what you want that's why I'm telling you to run some test.

The things you have to look for are "part copy", "inter part copy", and Peer variables, these tools are very helpful to build models that interact between each other but you have to use them carefully because sometimes they can give you some headache. Another things to take care of is using the same template to model your door. What I mean by that is that by using a model and then using save as to build a second one that you simply change dimension keeps all the numerical values of each surface and planes intact so that you can replace the first part with the second one in your assembly and solid edge won't mess up all your assembly relationship because He will recognize the same surfaces with very simple or no modification.

Also the more you use "part copies" and "inter-part copies" the heavier the assembly becomes and the longer the update time is.

I think that with SE V16 you have a strong software that will help you increase your workflow by making the kind of model you want to do but I just want to suggest you to be patient and warn you that it won't happen with a finger snap.

Good luck

Patrick

 

[fredericmenage]

Bellerophon,

you should follow patrick's advice. I just have a few comments to add:

1/ consider not using Excel since Solid Edge has a variable table. This will save you a bit of file management and will simplify the workflow.

2/ Don't use 'save as' when in your template assembly to generate another one. This will break the links that use the filenames. You should use the revision manager in Insight Connect instead. Ask about that during your training.

3/ Don't try to build a perfect parametric assembly. Build a good one with 80% of automatic links and keep the last 20% for manual updates.

4/ Regarding the cutsheets and hardware list sheets, consider using quicksheet as well as 'save as flat'. I don't think this step can be completely automatized though.

Fred

 

[Bellerophon]

Great! Thats exactly what I needed. glad you guys are so helpfull. I was hopeping noone would look down on me due to my lack of experience. I just ordered this book so hopefully that'll help get me well on my way.

http://www.cadcim.com/solid-edge-16/solid-edge-16.htm

 

[Bellerophon]

also a follow up question if I may. (copied from another forum)


how do I repeate a cutout every 8 inches on center? so if I resize the part it will adjust the number of holes accordingly



"Kevin Grayson" <kevin.grayson@engmeth.com> wrote:
>
>One way to accomplish this is create your initial hole and then create a rectangular
>pattern of the hole. By using the Fill Option, you can specify the x spacing
>so
>that as the part changes, the number of holes changes accordingly.

I gave that a try. It places the correct amount of holes but once the part (tube) is lengthened or the orig hole is moved the holes do not populate to the newly extended area. It also gives the feature the following error.

warning: some of the resulting features do not add or remove any of the material

Thanks for the help!

 

[fwc]

Hi

The message tells you that some of the holes are out of the part.

To achieve desirable results you'll need to create relationships between;
1. The part length and the rectangular pattern.
2. The initial hole and the rectangular pattern.

HTH

fwc

 

[PatCouture]

You are right Fred, don't use the save as option, but what I mean't by that is using as much as possible the same model don't start all over each times.

Bellerophon, Revision manager is very good for copying not only the model files but his corresponding drafting files in the same manners. I think you will use it a lot.

Good luck

Patrick

 

[kjoiner]

Bellerophon,

Like fwc said, it sounds like you need to place a dimension between the far end of the pattern rectangle and the edge of the part. That way, when you extend your part, it will pull the rectangle along with it and SE will add new holes as it can fit them in. I used patterns like that for alignment holes on machine cabinets we make that come in several different sizes. I constrained the 1st hole and let the pattern follow along when the machine changed sizes.

Also, let me know what you think of that book. I've been looking at it also.

Keep posting questions and update us on your project. Discussions like this promote thinking and a lot of times lead to ideas others can use for their own projects.

Kyle

 

[Bellerophon]

Thanks for the help and encouragement all. I've managed to come up with pretty much what I need, however I need the pattern to center itself on the part even after it resizes. Could someone take a look at my par file and let me know if I'm on the right track and how to center a pattern?

http://febr.us\Lee\window.par

Kyle, I'll be sure to let you know when the book comes in

Thanks
Lee

 

[kjoiner]

Bellerophon,

You can create the initial hole and constrain it to the mid point of your part. Then create your pattern toward one end of the part. Next, mirror the pattern about the midpoint of the part. You will need a plane at the midpoint of the part. Along that idea, it is helpful to constrain the midpoint of your part to the center of the reference planes when you start your model but if that is not possible, you can always create a parallel plane and place it at the midpoint. With the mirrored plane and your pattern constrained according the previous posts, your pattern will stay centered on the part and also add or subtract holes as your part grows or shrinks.

By the way, I was not able to view your part, but I'm making an estimate as to what you are wanting to do.

Kyle

 

[Bellerophon]

Ok, I thought that may be the way to go about it. I just didn't know you could mirror a pattern. I'll give that a try tonight. Oh and just to make things even harder (I'll try and make this my last question for the xmas break) Is there a way to do the following on the part I've been trying to make above?

Detect if the fill patterned holes fall within 4 inches of either side of the angle protrusion and have it automagically shift those 2 outermost holes back two inches? Or is this going to be a manually check and repair type of thing. By hand I suppose I would just suppress the two outer patterns and then replace the new shifted ones.

Sorry if these questions are too basic. I figure the more I struggle through my parts before the training classes, the more problem scenario's I'll be able to bring to class on CD.

Lee

 

[kjoiner]

Lee,

I'm not sure about having the dimension automatically shift (there may be a Visual Basic program that could do it) but you can probably use the sensors available in SE to alert you to a condition where the holes are too close to the edge. You would then manually change the dimension and the pattern would adjust.

Kyle

 

[Bellerophon]

Thanks Kyle, I gave it a try last night and I kept getting something about the Sensors Parent being lost. I think I may just have to deal with this one by hand.

 

[Irwinfletcher]

Not sure if this will do exactly what you want, but could you do the end cutout first (dimension it 4 inches from the end of your protrusion) then do the pattern as described above and constrain this to the end cutout yuo just did, and then mirror them both. The end result is that you get your end cutouts 4 inches from the ends of the protrusion and the pattern fills the length between them, centred about the middle.

 

[Bellerophon]

Thanks for the try Irwinfletcher! still no good though. It does do exactly what I'm asking it to do but still not quite what I'm looking for. The problem is it fills the area with the cutouts but it'll overlap the last patterned hole with the end ones if there's just enough room to. If I resize the part a little bigger the last patterned hole will sit right next to the end hole which blows the whole "every 8 inches" idea. I'll have to ask the boss on what he wants to do in this occurance.

 

[Bellerophon]

ok, my senses finally came to me and I took this approach.

Drew the pattern close to the end of the part, then used smart dimension from the end of the part to the end of the pattern. set it to 4 inches and it worked! I did this on a test part. however when I tried it on an identical part I'm using in an essembly, the smart dimension doesn't seem to effect the endpoint of the pattern. It doesn't matter what obsurd number I set the dimension to, it just changes the number but doesn't actually move the dimention. I dont know if its a bug or some sort of protection since the part length of the piece used in my assembly is linked to an excel spreadsheet.

heres some pictures to help explain

working on part not used in assembly

http://www.dcsportbikes.com/forum_i...cd357-a59e-496c-86d8-bd46e34eb001_working.jpg

not working on part used in assebly

http://www.dcsportbikes.com/forum_i...a9-d818-4aab-96ae-300da05b74d7_notworking.jpg

smart dimension set to 4"

http://www.dcsportbikes.com/forum_i...b-3548-4243-af5c-48283e4bf846_notworking2.jpg

smart dimension set to 40"

http://www.dcsportbikes.com/forum_i...f-7b8b-4b62-91db-9fcffd0980c4_notworking3.jpg

 

[fwc]

You may want to try this. However, you'll need to link SE to Excel.

The followings are done in SE file.
1. Since the hole at outermost position varies, do not include that hole in the pattern.
2. You should add a new hole for the outermost position.
3. When adding the hole, dimension its center to the mid-point of the angle or center of the initial hole. Link this to G in Excel file.
4. Pattern the initial hole, use Fixed Pattern Type.
5. Mirror the pattern and the outermost hole.

Create the followings in Excel file.
A= 80 in (Link this cell to the length of the protrusion in SE Variable Table.)
B= 8 in (Link this cell to the pattern spacing in SE Variable Table.)
CC= FLOOR(A/B,2)
E=(A-(B*CC))/2
F= CC/2 (Link this cell to numbers of occurrence in SE Variable Table.)
G= IF(E<4,F*B-2,F*B) (Link this cell to the dimension (No. 3) in SE Variable Table.)

To link the cell to SE;
1. In SE, Go to Tools>Option, select Inter-Part tab and check Paste link to variable table.
2. Save the Excel file.
3. Copy the cell in Excel.
4. Select the row in SE Variable table.
5. RMB and select Paste Link from the Shortcut Menu.

Change the value in A to see if it’s what you are looking for.

HTH

fwc

 

[Bellerophon]

I'll have to give that a try fwc, thanks for all the effort! why did you use the CC row instead of C?

 

[fwc]

I couldn't name the cell (in Excel) to C that's why I name it to CC.

Keep us informed of your development.

Regards
fwc