Hello, my question is "relatively simple"... How do I get a flow sheet from my modeling on SolidWorks?
The challenge : I am a carpenter and I proceed SolidWorks 2018. Rather a beginner in CAD I try to optimize the time I spend on it as much as possible. To do this, I would like to create a flow sheet that takes into account any changes to my parts and that is generated automatically. All this without using external software such as Excel... So I try to extract the overall dimensions of each part!
Track :
1- I think I can use personal properties to extract the necessary information... but my knowledge is lacking in this area. Before I start researching and watching hours of tutorials, do you think this would be a solution?
2- If track n°1 doesn't work, I'm desperate and I'm turning to you for a sketch of a solution!
Don't hesitate to ask me for more info!
Thank you for your attention and your contributions.
I would start with the use of SW sheet metal and /mechanical-welding tools (a board is a kind of sheet metal).
You will then have access to the information you are looking for. For the speed, look at the "visualization cube" function (from memory).
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By doing mechanical welding, you can bring out all the lengths necessary during the drawing (by also inserting the marking bubbles).
In the drawing: insert: --> table --> list of welded parts.
When the table is installed, see attached image to make the column long.
I hope this can help you!
capture.png
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Hello
I don't answer your question directly, but you should know that there is a specialized module for SWOOD and other possibilities to go faster and spend more time in the workshop.
Here is the link to inform you
And a video to inform you too ;-)
There is also the option to use the free driveworks Xpress tool which is very useful too. Here is a use in a carpentry context.
Kind regards
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Thank you for all these contributions! I'll check that out... All that remains is to get started^^
In my research I saw that the dimensions of a part were specified in the table of "equations, global variables and dimensions". Wouldn't there be a way to get this information via a custom property and include it in my planting later? (See attached the imp screen.)
Thank you so much for your time!
imp.ecran_equation_variable_globales_et_cotes.pdf
No need to go through custom props, you can display the dimensions of the model directly in the drawing.
Quick question, did you have SW training or did you just do self-training?
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Hello @stefbeno,
I don't have an SW background, I have a very light background in CAD but which allows me to easily understand how SolidWorks works. In addition, SolidWorks is a very flexible and "intuitive" software... So with all the support that the internet and the community provides, I think this will be enough^^
However, I thank you for your interest!
I think I've found the solution to my problem! I'm currently setting it up... I will then test it and come back to post the solution on the topic to help the rest of the community.
See you soon
Let's say that for the basic operation, indeed you can be satisfied with self-training but as soon as you attack advanced functions, it is profitable to follow a real training (it can be 2-3 days so not necessarily an exorbitant cost).
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So here is my method for making an automated debit sheet. I present you a simplified version because I have created another sheet with equations for the notion of raw wood and finished wood dimension . This flow sheet will be updated with each reconstruction and takes into account the changes to the parts. The most important thing is to make these coin quotes right from the start:
1- Create a custom property form using the editor that is in the SolidWorks Tools in the Start menu. Install the text boxes and apply it for parts only. Other options can be added depending on your needs (see attachment)
2- Save your form in a dedicated folder and have it recognized by SolidWorks via the options: Option > File Location > Customize Property File.
3- In the pane on the right that contains the home you will also find the forms of the customize properties. Select your new form that you would have named "debit sheet" and select the dimensions that can be controlled (for complex shapes) by clicking on the box of your form and then on the odds lines which puts your value in the box. Do the same for the rest of the dimensions of interest and don't forget to apply your form.
4- Open your drawing and incorporate your part or assembly. Go to annotation > select table > BOM table > select your view and paste your table.
5- Customize your table by double-clicking on the letters of the columns > a box appears and selecting the personal properties > the item of interest.
6- Repeat step 5 until your table meets your expectations
7- Save your table by right-clicking > save it as > folder dedicated to your SolidWorks custom settings > have your table recognized via Option > file location > BOM template
Do not hesitate to contact me for more info;)
notice.pdf
That's what I thought, a table of welded mechanical elements was enough but much less complex.
@stefbeno unfortunately I don't have this option on my SW prenium 2018! My bad, Maybe I didn't activate it!?
The mechanical-welding and sheet metal functions are part of SW standard so you have them.
This is the problem with the "adaptive" interface of the software, try to right-click somewhere in the ribbon to bring up the other available tabs.