Best way to call out material of a model in a drawing note

SOLIDWORKS How To Questions
1

We are considering how to call out the material on our drawing. We would like to set up a system that does as many things for us automatically as possible to reduce human error. We are using PDM standard and SolidWorks 2023 SP 4.0.

It is possible that I am overanalyzing this. (But would I still be an engineer if I didn’t? :smiley: )

We design plastic parts. These parts are often tooled and molded in China. We have noticed that our notes are not always followed and suspect that language may be part of the problem. (We have limited control over supplier selection so often end up with different suppliers.) To solve the language barrier, we plan to have a translated copy of our notes on the last sheet of our drawing. So, our standard plastic notes will be on the first sheet in English with one note in Chinese saying that the last sheet will have the Chinese translation.

We do not plan to translate the material since it is usually a particular supplier and grade. We need to call it out on both the first and last sheet. We are considering a few options, and I would like some opinions on which is best and the risk with each.

Right now, we often assign a generic material to our model such as PC/ABS. Our parts have a material property set to “SW-Material@.SLDPRT” . Currently, we call this out in the notes on our drawing as MATERIAL: $PRPSHEET:“MATERIAL”. We often then add some additional information such as the material manufacturer and grade. So the note ends up reading:
MATERIAL: PC/ABS, COVESTRO, BAYBLEND FR3010, BLACK
(MATERIAL: $PRPSHEET:“MATERIAL”, COVESTRO, BAYBLEND FR3010, BLACK)


Ideas in consideration:
Create a DWG-MATERIAL property in our drawing and use $PRP:“DWG-MATERIAL” in our notes instead of $PRPSHEET: “MATERIAL”.
Have only the additional information in the DWG-Material property so our note looks like: MATERIAL: $PRPSHEET:“MATERIAL”, $PRP:“DWG-MATERIAL”.

We can set the DWG-MATERIAL property as “SW-Material@.SLDPRT”, , but I do not know a good way currently to bring “SW-Material@.SLDPRT” into the drawing property. Any suggestions? Should I even worry about this?

We could just manually enter the material information in the DWG-MATERIAL property. If the assigned material in the model and the drawing did not agree, this would not cause problems downstream at this time. (There isn’t material information in a STEP file anywhere is there?)

An additional complication, sometimes our drawings are of assemblies rather than parts. This means that we have to make sure to copy the material from the part into the assembly if we are using $PRPSHEET.

We currently keep the revision of the model and the drawing the same.

After writing out this explanation, I am leaning heavily towards just adding the drawing property DWG-MATERIAL and using that property in our notes.

I do have some ability to write macros so we could set up something helpful there. We also still use the property tab builder (even though we have PDM) and I could put some options in a pull down so users could select a material.

We do have a good checking process for our drawings, so many human errors get caught by the other humans.

Thanks,
Carrie

2

I cannot suggest anything regarding the PDM, but I would recommend two things.

  1. MATERIAL: PC/ABS, COVESTRO, BAYBLEND FR3010, BLACK or Engineering Approved Equivalent, and then make sure you have a clear and easy process in place for your molder to apply for an equivalent material permission. This should list the part number, your specified material, their requested substitution, etc. It should also include the outcome: Approved or Not Allowed (with reasons why not). This then becomes a reference library for future equivalency requests which will speed up the processing.
  2. Have your material suppliers (Bayer, et al) provide the Chinese specification. Use that on the translated material note along with 或工程批准的同等 (that’s what Google Translate provided for "or Engineering Approved Equivalent).
3

I always keep properties in model. Drawing just display those properties.
Assign correct material to model or setup material properties in model.
The model should contain everything (or as much as possible) required to make it. So it can be reused.

We have noticed that our notes are not always followed and suspect that language may be part of the problem.

I don’t think so. This happen in all suppliers. Even in our own shop.
If they can’t read english, what make you think your translation is better? Do you have someone that worked in China and know the lingual? There are lots of technical slang that are difficult to translate.
Even if you got someone, you have no way to confirm their translation is correct :wink:

I don’t know if China use Imperial or ISO standard. Or even their own.

Even translating steel standard is not simple.

Also there are lot’s of stories of inspection sample are great, production looks nothing like that.

4

We are also planning to use the note “NO MATERIAL SUBSTITUTIONS ALLOWED” because we have had a major problem with a supplier (that we are going to steer away from in the future) picking a generic PC/ABS and trying to color it rather than buying the very specific grade with the color code included that was specified. o[
We are also saying “MATERIAL CERTIFICATION REQUIRED WITH EACH PART ORDER.”

Though we should create a form for getting approval for alternate materials.

5

Frederick_Law We do have a Chinese speaker on staff and have a couple of other resources, including our notes having been translated and shown in a recent DFM document.

Getting parts that are different between the samples and production is it’s own special challenge.

My concern around using the model property is making sure the right model property is used. We usually use only one model per drawing, but there is risk if we have any molded in hardware and use an assembly, that some of the views could use the part rather than the assembly. I don’t want us to accidently end up with something that reads differently between the first and last page. (Though we will have to be very careful anyway, so maybe this is a worry I should drop.)

Are you keeping your materials database in PDM?

6

I’m Chinese, from HK.
So my Chinese is different then China and Taiwan Chinese.
I didn’t work in HK. So I can’t say I’m fluent in manufacturing Chinese lingo.

Translate this: 士巴拿
It’s a very common tool most in HK know what it is.

Didn’t use PDM in SW.
Materials were setup in SW. Don’t remember if that can be share. You may not want material name to be so long.
Inventor use material library which can be in Vault for everyone.

In some company, they assign their material number and has a document for that material’s spec.
Maybe you can follow that.

7

That’s interesting. I used several different translators and I got:
士巴拿 translates to English as Spana, Shbana, the Basna, Sparna

I assume it means a spanner wrench. Frederick_Law, what do you say it is?

8

Right now, we do have the materials database in PDM and it is at a status that engineers can check it out to write to. I don’t know if anyone has tried adding materials to it since it moved into PDM. It was on a network drive until our PDM server moved to Azure and we couldn’t to our network drives while using PDM. I think that’s fixed now, but I’m not sure I want to bring it back out of PDM. We have to map the network drives every time we log back in.

9

oa

Correct.
There are lot’s of words, terms which doesn’t exist in other language.
So we just use the sound and replace with Chinese character that sound similar.
See bar ner.

10

We settled on using the property MATERIAL in our model and we’ll call that out on the drawing using $PRPSHEET:“MATERIAL”.

11

i’ll start here to avoid starting a new thread for similar topic.

I havent had to make drawing templates for 15 years. Seems to me if my template has $PRPSHEET:“MATERIAL”, the material should show up in that box when I make a drawing from the part. Do I need to have a custom property for that? SW doesnt pull that from the part info if i have a material in there?

Same for Mass and File name…. Thanks!

12

Use $PRPSHEET:"SW-Material". This will use the material defined in the model.

Similarly:

Mass: $PRPSHEET:"SW-Mass"

Filename: $PRPSHEET:"SW-File Name"

If you want the path as well, you need:

$PRPSHEET:"SW-Folder Name"$PRPSHEET:"SW-File Name"

Also, if you haven’t made a template in 15 years, you need to read this (emphasis mine):

==================================================================

Solution Id:S-071805

Product:SOLIDWORKS Professional 2016

Created:8/18/2016

Technically Reviewed Date:1/4/2017

Area:Save/Open

Sub-Area:

Question:In the SOLIDWORKS® CAD software, how do I determine if I am using an old template?

Answer:Making sure that you use the correct template version for your version of the SOLIDWORKS® software is fundamental in avoiding unexpected behavior in the Sheet Metal, BOM, Cut List and other environments.

There is no tool available in the user interface to check the template version. One way that you can do this is as follows:

1. Create a new part or assembly.

2. Select the ‘Top Plane’ in the FeatureManager®.

3. Right-click and select ‘Properties’.

The ‘Date created’ field provides information about the creation date. If the template is very old, consider replacing it with a new template from scratch.

As a best practice, you should not save an old template in the latest version of the software. If you create a new part from an old template and then use the ‘Save As’ function to replace the template in the latest release of the SOLIDWORKS CAD software, some internal data does not update properly.

====================================================================

Extensive discussion here:

13

i’ve tried using those that you listed. i have to make a custom property in the part file to get the material and the weight in. does SW not just do this automatically if i have a material defined??? i dont ever remember having to go into properties and create a custom property every time….

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14

oohhhhhhhhhhh…… i bet you i made a custom part template that has those in it, and then used that part template for everything.

”I see, it all comes back to me.” -the blind man peeing into the wind