Hi,
Please bear with me, I am relatively new to Solidworks!
I have this arm as a part, now I need to create an additional part that will accurately fill the holes outlined below:
Arm part file: DJI arm - RED.SLDPRT - Google Drive
Any suggestions?
Cheers
Hi Alastair,
If you create a reference plane on the planer faces either side of the holes, you can then use the intersect tool (with the option create internal regions selected). This will allow you to select which holes you would like to fill and which ones you would like to keep. (see image)
Hope this helps.
Kieran
I should also say you may need to use the combine tool afterwards as for some reason the merge entities option does not seem to work in the intersect command.
Kieran,
That's awesome and exactly what I was after. Is there a way to create individual part files from each of the 'plugs' (1-4 on the below image)? I need to 3d print each of the four plugs to put into an existing arm.
Big thanks for everyone else who chimed in, Solidworks has a great community!
Cheers,
Alastair
Hi Alastair,
I'm glad that helped.
You should now have a 'Solid Bodies' folder near the top of your design tree. If you click on each one of the bodies you will be able to see which body they relate to in the graphics window. Once you have found the ones you wish to have in a new part, you can simply right click on each of them and there is the option to 'Insert into new part'. (see image for reference)
Kieran.
Hi Kieran,
Thank you so much for that helpful reply. Worked like a charm
Have a great day,
Alastair
I am curious - how did you manage to do all of that work without dimensioning your sketches?
When I add the missing dimensions they come out perfect.
What is the workflow to get that to happen?
From the looks of things I am guessing feature recognition was used
Ah, I guess that could be it.
Whenever I use Feature Recognition - I only convert the features that I actually need to change - and then make the changes with dimensions.
I was provided the original part by a friend so I'm not sure of his exact process
Alastair
Maybe it will be usefull
1-Knit limits
2-Uncut surface to fill
3-Extend radii surface (2 places)
4-Extract sketchs for do extrusion (2 places)
5-Extrude to surface and join (2 places)
6-That's all
Hi Alastair,
You can use delete face feature. Attached are part in which I used Delete Face feature.
Manish
Just to note, the Delete Face / Patch feature can do more that one patch in one feature. I had assumed one needed a separate feature for each patch, and then was happy to discover than one feature could do multiple patches. In Alistar's case, all four holes can be filled in one Delete.
Dwight
Alastair
Delete Face / Patch works great.
Dwight
Crap, by one minute.
It has another way too see it.
RH
LH
I think this one is an easy way to you
It's a better choice
Its a nice technique but I believe the idea is to create a separate part that fills the holes?
Hi Alastair,
I'm glad that helped.
You should now have a 'Solid Bodies' folder near the top of your design tree. If you click on each one of the bodies you will be able to see which body they relate to in the graphics window. Once you have found the ones you wish to have in a new part, you can simply right click on each of them and there is the option to 'Insert into new part'. (see image for reference)
Kieran.