CAD Forum

Hello

So I want to embed my part shown here into a block and do a three way split for making a mould for carbon fibre layup. I vill 3d-print the three parts and clamp them together to make a compression layup after wetting out the carbon fibre.

I have a reference plain set up in the middle of the tube/tab and in back of the half tube going perpendicular to the first plane.

So how would I go about this, using the mould tool in solidworks(that I never used before) or using the cavity command and split feature command two times?

Terje

Or just use surfaces, subtract part from a block and split with the surfaces you created. Should take a few minutes.

Yeah, don't use the SW mold tool, just make splitting surfaces.

Hello
Thank you both, so I did not see your replays.
I've been trying out the mould feature in the meantime, I've kind of got it working, but I need the black part split down the middle to, parallel to the protruding tap. Maybe I can just make a plane and split it that way, or can it also be done ine the mold tool?

Terje

Now that you have the black part you could do a split part feature on that to get both halves.
And same as previous comments, the SW mold tools are a not ready for prime time feature.

Ok thanks, I will do that.

Yes one should believe the feature is developed for a reason.

So is there anyone in here that have experience with laying up carbon fiber cloth in such a small form, will it be doable with this kind of tre way compression molding? Any recommendations for a forum on this?

Terje

Worked like a charm!

I have only done composites on a simple hobbyist level, but I haven't seen a mold approached this way. I don't know the scale of the part, but that tab looks like a problem if you are planning on using cloth, unless you are going to make that separately and then bond it in. Given the amount of work I think it will take to get usable mold surfaces off a 3d print, I wonder why you don't want to make your mold with more traditional methods.

We made molds like this at my last job, but they were always aluminum. The tabs were part of the layup.

I wonder if you can get the clamping pressure required using plastic.

Thanks

As you mention, the tab is the reason I've made the mold this way, I don't think it's possible to lay up the fibre in traditional way and get the cloth down i the tab, but I really don't know, this will be my first attempt at carbon fibre part.

I contacted Easy Composite and they advised me to make the part in two pieces and then glue them together, but as it will also be a cosmetic prototype show part I think I will try this rute first. The tab is 10x20x20mm, so I was thinking, can I use some core material and put it between the two halfs when I close the mold to get the 10 mm with? The finished part most take a lifting load of minimum 25KG before I see any crackling between the stem and the tab.

As for clamping strength, I was thinking of putting the printed parts between 4 pieces of aluminium before clamping. I will also make some holes for dowel pins to align the parts. Yes of course aluminium would be better, but I only have a 3d-printer, a Markforged two, so I think the mold can be really strong printed in Onyx and fibre reinforcement. I have been banging my head to come up with a design to just print the part with carbon fibre reinforcement as my printer can do that, but I can't find a good way to line up the layers(the part of the design where the forces are acting up). If only one could print in three dimensions aligning the layers to the curved faces.

But as I said, it's my first try with carbon fibre so I'm open for all ides, and even to outsource it

Terje

I don't see any reason the tab couldn't be integral to the part. You just have to work through the layup schedule and figure out how to make it work. We used pre-preg, so it might be more complicated with a wet layup. Our carbon guy had done test layups of all of the materials we used, so he knew if he had a 1/8" tab how many layers were needed to hit that thickness when compressed and cured.

When we did a tab like that, the pocket for the tab was only in 1/2 of the mold. The other side was flat. (Your parting line will not be on center.)

You might also consider investing in a small vacuum pump and some bags. That would make it easier to apply even clamping pressure.

Thanks for the tips

I will make a model of that and see how that will work out for me, and oh yes maybe use a vacuum bag to.

So as you can see, this time I used the manual method with combine and surface cut, but then it doesn't mask of the hulls like it does in the mould feature.

It seems like I have a problem with the fillets when I put the cut flush to one side, maybe I should go one mm in into the tap, do you know where your coworker did put the cut, or maybe he didn't use fillets?

temo wrote: ↑Thu May 12, 2022 6:25 pm It seems like I have a problem with the fillets when I put the cut flush to one side, maybe I should go one mm in into the tap...

Could you add the fillet feature after splitting the mold part? That might help resolve the issue, maybe.

Hello again

So I'm trying to save out the bodies to an assembly, but when I browse for the file location and click save, I get this error message that doesn't make any sense. My Solidworks version 2021 is installed at default location on the c:drive. I've tried different locations on different drives, but get the same message. I've looked into default file locations in solidworks settings, but can't find any who refer to the location on the error message. When I look at the menu for Save bodies I see there is no option for override template settings for assembly, just for parts, but in the help menu it shows that you can override both parts and assemblies location.

Any tips on how to get by this, so I can save the file?

Thank you, well yes I could, but then I think I would be without fillet at one side

To get the radius on both sides split the blue and green part so it is down the centerline of the part. The feature forming the thru hole can either be all on one side or equal amounts on each half. As far as the save issue, based on the screen shot it appears your assembly file doesn't have a name, if it is trying to save a file named .sldasm. Just a guess.

Also, maybe it's just me, but if you turned off the "real view" feature before creating the screen shots it would be easier to see what is going on with your parts.

We added fillets and drilled holes post processing. It was not part of the mold.

Thanks again everybody

Yes probably best to add fillets later and I also made a version where I split the mould down the middle.

No problem, I'll turn off realview in the future, but regarding the missing name, that's because it's still a part with 3 solid bodies that I want to save out as an assembly, but it wont let me name it. I've tried just typing inn the name and browsing for the catalog, but to no avail. I've tried with old and new parts, same same. I can not understand why that file location is showing up when I save, possible looking for a template, but that's not the template directory, and I never saved any files there before.

What a nightmare

So by this lead here: https://r1132100503382-eu1-3dswym.3dexp ... 3oUKgXQAuA I manage to resolve the issu after a cople of hours trying.

Basically save out the three parts without using the assembly option, then open each part separately, then do a save as on the part overwriting its name. Go back again and do a new "save bodies" command, give new names to the three parts and the final location you want for your new assembly and name the assembly.

As you also can see now the feature has the missing link to the file location for the assembly location. Hopefully next time it will work without any kinks.

temo wrote: ↑Fri May 13, 2022 11:17 am What a nightmare

So by this lead here: https://r1132100503382-eu1-3dswym.3dexp ... 3oUKgXQAuA I manage to resolve the issu after a cople of hours trying.

Basically save out the three parts without using the assembly option, then open each part separately, then do a save as on the part overwriting its name. Go back again and do a new "save bodies" command, give new names to the three parts and the final location you want for your new assembly and name the assembly.

As you also can see now the feature has the missing link to the file location for the assembly location. Hopefully next time it will work without any kinks.

Some kindof workaround is to rename original SW name(of part) and than save bodies works

temo wrote: ↑Fri May 13, 2022 11:17 am What a nightmare

So by this lead here: https://r1132100503382-eu1-3dswym.3dexp ... 3oUKgXQAuA I manage to resolve the issu after a cople of hours trying.

Basically save out the three parts without using the assembly option, then open each part separately, then do a save as on the part overwriting its name. Go back again and do a new "save bodies" command, give new names to the three parts and the final location you want for your new assembly and name the assembly.

As you also can see now the feature has the missing link to the file location for the assembly location. Hopefully next time it will work without any kinks.

If the save bodies command was not working for what ever reason probably permissions issue (if right click on the solidworks icon - properties - compatibility - tick run this program as administrator). I'm 99% sure that would fix your problem.

Anyway regardless, in the absence of save body (and there are some issues with it other than save bodies file bug) the way to go would have been - insert the entire assembly into each part and delete unwanted bodies. It would have kept the link to the original file and hardly adds any weight to the new parts. Believe it or not this way is way more stable and more adapt for future modifications to the original split file without causing a total meltdown.

Lapuo wrote: ↑Mon Jun 06, 2022 8:17 am Some kindof workaround is to rename original SW name(of part) and than save bodies works

This, or save part the number of occurences you need(body count, in this case, 3)
Each occurence, use "Delete/keep body" on the appropriate body.
Build assembly using 3 parts inserted on origin.