showing material to be removed 9

[Yogibear]

I had the question posed to me how to show, on a drawing, the material to be removed. For example let's say you start w/ a rec. bar stock 12" long. Then you cut that down to 8". How do you do a drawing and show the 8" in a solid line type yet show the 4" that was removed in phantom or someother linetype. I know you could just draw the lines into the drawing to show it but I was curious if that could be done in the model somehow. I thought a split line might do it but I can't change the linetype after the splitline.

SW 2006 SP3.0

 

[ctopher]

You shouldn't show it. Show the finished part. The material note will indicate the material size made from.

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[Heckler]

You don't want to put limits on your purchasing dept by specifing raw material lengths. Let them buy the material in any form that's logical to the part being made or other parts that use this same material. Sometimes they buy rems or have to buy full lengths but that's not really your concern.

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 5.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NVIDIA Quadro FX 1400
o
_`\(,_
(_)/ (_)

Never argue with an idiot. They'll bring you down to their level and beat you with experience every time.

 

[ctopher]

I agree 100%. The dwg should show the final product, let purchasing work with the machinist to pick the appropriate size.

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[mncad]

This is just a rant and will probably make people mad, but here it goes anyway. Why debate the guy on if he should show the material on the drawing or not, that isn't what he's asking. Shouldn't we try to answer the question asked instead of beating the guy up for asking it? Not everything has to be done, or can be done to drawing standards, sometimes you have to do whatever needs done. I've never tried what asking about, but I will look into it a little tonite.

mncad

 

[ctopher]

Here it goes...
No, you can't do it in SW. The reason, not standard practice.

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[ShaggyPE]

Within the context of an assembly, look into creating a second part that is the material stock size. Using the mold tools (cavity), remove the finished part geometry from the piece of stock. Create the view in your drawing from the assembly of these two parts (finished part and material stock). When in the drawing change the linetype of the material stock to phantom.

This will almost achieve what you are looking to do. You may have some issue with the linetype of some of the hidden lines, but you may be able to change those individual edges into solid.

-Shaggy

 

[MN5520]

We handle this in the following manner.

1. Create the part model to finished size.
2. Create a configuration of the part (in our case we call it a lathe or mill configuration)
3. On the new configuration, use the "Move Face" feature (found on the "mold tools" tool bar)
4. Save the configuration
5. For the drawing, Sheet 1 is the finished size, sheet 2 (or whatever you choose to name it) is the configuration with the added material. Or optionally you could create a view of the secondary configuration on drawing sheet 1.

I agree with mncad and his rant by the way.

Hope this helps.

Brian
SW2006 sp3.4

 

[StefanHamminga]

If you want a step by step guide to constructing a certain drawing you could model the part as a whole (I do this on some weldments, when they want, for example, an internist to build a certain part), then use configurations to 'step' through the construction process (unsupressing the next features for the next step).
Then use a drawing sheet for each configuration and you have a step-by-step guide to building the part the way you want.

PS. Be very sure to build the model the exact same way you want your part build!


Stefan Hamminga
EngIT Solutions
CSWP/Mechanical designer/AI student

 

[ctopher]

I'm sorry if I come across a little harsh today. Having a bad day.

I'm going for a walk...

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[handleman]

I agree strongly with mncad. The question asked how to accomplish a task. If you don't think that task is worthwhile, fine. Even *suggest* that in your *opinion* what he wants to do shouldn't be done. But don't say that it *can't* be done because it's not "standard practice". If you're not aware of a way to do it, say as much, and wait for someone to post who knows how.

OK, rant over. Here is how to do it. It's a bit roundabout, but it works.

1. Model your part with two configurations - one as raw material and one as the finished part.
2. Insert the model into a new assembly. Make two configs of it, each one referencing a different configuration of the part model.
3. Make your drawing from this assembly. Each view should reference the assembly configuration referencing the finished part.
4. Add alternate positions referencing the raw material configuration on any view for which you want to show raw material.

Note that this does add all the limitations of alternate position views (no cropping, no broken-out sections, etc).

-Josh

 

[wgchere]

I'm afraid I have no idea how to do it. but I want to say: it is standard practice for Altered Item Drawings. The standard for types of drawings says to show the original size in pahntom if any material was removed. Bravo to Yogibear for reducing it to a simple example instead of a real world one like this:

"We have a power supply we buy which works electrically, but doesn't fit our assembly. So we remove the mounting plate and drill some new holes and trim the size. It isn't rectangular, so we cut off .85" from one side and remove a 1" x .75" tab on the adjacent side. Then we add a 4-hole pattern for mounting and cut a few notches on the side. How do we show the material we removed..."

And the responses would be:
"That's too complicated. We need a picture"
"Why don't you buy one that fits?"
"Have you already done a search of the site? I think a similar problem was discussed here in 1998. Do your homework."

 

[Heckler]

Why debate the guy.....easy we can all learn something. I still agree with Chris regarding standard practices. If you place that type of control on a print telling them what your raw material length should be.....your part price just increased. It doesn't add value to the end product. But if that's the way your company does business then you have the correct answers above.

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 5.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NVIDIA Quadro FX 1400
o
_`\(,_
(_)/ (_)

Never argue with an idiot. They'll bring you down to their level and beat you with experience every time.

 

[CorBlimeyLimey]

A simpler alternative;

1) Create the model of the finished length part.
2) Add a sketch (to the model) representing the removed material. The linetype can be set in the sketch and the sketch can be set to Hide if necessary.
3) In the drawing view, make sure the sketch is set to Show.

This way the "removed material" information always stays with the model.

TFIF tomorrow.


Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091

 

[CorBlimeyLimey]

And the responses would be:
"That's too complicated. We need a picture"

What's wrong with asking for a picture to clarify the problem? Often a question is poorly worded, ambiguous or just plain unintelligible. It takes very little time to upload a screenshot to an image hoster. Isn't it better to be sure of the question before throwing out misleading or incorrect solutions?


Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091

 

[ctopher]

I agree CBL. Sometimes staring at a computer screen all day, I just can't make sense of some wording. A picture comes across a lot more clear.
I still hold to my opinion. Show the dwg as the final product. List the make from material in the BOM or a note. If the make from material/part is a unique shape and the finished part is unique to the M/F and is oriented as such, then it is OK to show the relation in a view. I would draw a sketch outline in the part's dwg view. The sketch can be dimensioned in the view to the part to make it constrained and then the dim's hidden.

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[brengine]

We do it the way CorBlimeyLimey described 3 replies above. To add to that, if you don't want to rely on other Users to leave Sketches as Shown, you can...

1) Show the sketch
2) Select the sketch lines and do a convert entities.
3) Hide the sketch/all sketches.
4) Change your Converted Entity lines to construction lines, or to some other line type if needed.

Ken

 

[pdybeck]

Model the stock material. Insert as a base part and machine away what you want to. Perform a geometry compare using SolidWorks Utilities. Save the results off to a file. Save that file as a parasolid. Go back to your machined part and insert the geometry compare parasolid into your file. Using the new mate tools in part files, locate the geometry compare bodies over top of the machined part. Create a config where the bodies are suppressed, or unsupressed. Reference both configs on the machined part drawing.

Pete

 

[Yogibear]

Wow, that's a lot of responses for just overnight. Thanks mncad for seeing the question. I agree that this is not a good thing to do and I don't do it but the guy was told to make the drawing exactly like the paper drawing that he had in front of him. We do this sometimes since we are part of a Japaneese company and don't have access to the original cad file.
Thanks for all the input and glad I could open a can a worms for you all.

 

[CorBlimeyLimey]

Yet another alternative;

Create a multibody part. The "removed material" can be modelled not "merged". Then in the drawing simply change the linetype to suit.


Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091