i have a bracket (currently an assembly with multiple fasteners and parts) that i need to put in all the corners of a weldment. The weldment is all 90 deg corners and such so if its possible i would think this is a pretty easy use case. I have been trying different ways after putting the weldment in an assembly.
Will it not allow you to pattern the component?
If it is in a part file, try checking the box for bodies
its a weldment that has been placed in an assembly and i need a part to be patterned around it.. i tried the pattern driven component pattern but its kinds useless because there is like only 1 other corner that it could pattern on. I put a hole wizard hole in every corner just to locate the bracket to see if it would work but it will not go outside the plane that you set as a driving feature even though it's all over the part. although that command does work really well for other stuff.
Have you tried a linear or circular component pattern?
Lets see a model file or some screenshots plz.
This is probably a pretty simple question to answer but we're all going at it blind
Hello,
Can you post some screen shots?
Or upload your files?
This should help improve the quality and quantity of replies.
Kevin
Just from the top of my head without knowing the situation better. Would it be manageable to use 'Offset Entities' to create a line around the weldment that you could then use to pattern those brackets?
-Topi
As others have said, it's difficult to offer much help working blind, but is your weldment symmetric, and has planes going through the center? If yes, you could probably use two Mirror features to place the brackets.
So I have around 25 of these brackets to put into each corner of 5 different models (so minimum 375 mates and hole wizard holes for the bolts is 500) . Mated the back face to the crossmember then the other face to the post and then selected the midpoint of the cross barrier and mated to the plane. what would be freaking amazing is to make the hole wizard holes in the posts for the two bolts and the two holes in the crossmember as well.
I have a feeling this is just to much to ask for, but hey, maybe there is a chance.
It will depend on the geometry of your frame. If it is square you could probably put one bracket-hardware sub-assembly in and do a circular component pattern. Then mirror to get the brackets on the other face of the posts?
If your bracket will always be in the same location on your cross member it may be easier to make an assembly out of the bracket-hardware & cross member so when it is located the bracket is too.
figured out how to do this, i mean i still have to do mates but its so much easier. thanks for thelp. good thing to know in my back pocket
so i'm running into a little bit of a wonky problem trying this. I name the matereference the same thing in each part. then i do the same order of mates in each part. i do it once and it works but when i want to do it on another side it doesn't work with the same mates at all. i did it all the same on part of a product in a bunch of different direction and it worked fine, but once i got over like 5 of them it would stop working. i read all the solidworks help i could find and the stuff i am finding online is for circles and stuff that looks really easy. so, do you have any other resources or anything you could share to make this work better.
Create a subassembly with all of the common hardware along with the bracket and change the Properties of the Default configuration to set "Cchild component display when used as a subassembly" to "Promote". The bracket and hardware will show up on the BOM like normal and the subassembly will not be shown on the BOM.
Ben Langdon wrote:
So I have around 25 of these brackets to put into each corner of 5 different models (so minimum 375 mates and hole wizard holes for the bolts is 500) . Mated the back face to the crossmember then the other face to the post and then selected the midpoint of the cross barrier and mated to the plane. what would be freaking amazing is to make the hole wizard holes in the posts for the two bolts and the two holes in the crossmember as well.
I have a feeling this is just to much to ask for, but hey, maybe there is a chance.
Do you mean like if there was a Hole Wizard feature you could use in an Assembly, so you could put holes in multiple Parts with one operation...
... and have the holes carry over to the Part files?
can i do that hole wizard with them not being on the same plane?
Ben Langdon wrote:
can i do that hole wizard with them not being on the same plane?
I don't understand what you mean about them being on the same plane. Does this screenshot and the attached example help?
when it asks you in the position tab you usually only get to select 1 plane and there for i would have to have a bunch of hole wizards. which is not terrible but it would be cool if i could select holes on different planes
Hole wizard holes can be on any number of faces - you just need to use a 3D sketch for hole placement.
2018 SOLIDWORKS Help - Hole Wizard Overview
O.M.G I am truly a noob.
wow, just wow. this changes my whole workflow.
i have so many parts with like 30 holewizard features with the same fastners but since they were on different faces i made each a new feature.
you may want to look into making the bracket a "smart component" - it could know to bring in the hardware and add the holes to mating parts.
Hello,
Since your bracket is bent, I'd add the same corner one as another insert for the common corner pairs:
Then mirror twice to get the four corner pairs.
Linear pattern up & down if they are levels at the same frame dims/orientation.
Kevin
EDIT: Even though my fake frame was made about top/front/right, to illustrate, I created two mid-plane planes by selecting the each pair of opposite outside frame faces and used these for the mirrors.
So i ended up not doing it in a pretty way but it was a lot easier than copying each subassembly and then manually doing 3 mates, ie clicking on two faces and than coincident mates.
Copy with mates got the job done a lot faster. first time using it and learned a new thing today.
Hey Ben,
Do you know what promoted assemblies are? They could save you a lot of trouble in cases like these imo
are you referring to this?
https://forum.solidworks.com/thread/47173
Under configuration properties for an assembly file there is a Bill of Materials Options set - The three radio buttons are show, hide, and promote for "Child component display when used as a sub-assembly"
When this assembly is used in another assembly then the BOM will automatically show the sub-components as existing at the assembly level and not as sub-assembly components.
The other route is as you showed in your attachement. When A indented bill of materials is added, but then where the assembly shows up with its sub-components you "dissolve sub-assembly" within the BOM. This "promotes" the assemblies components up one indent in the tree 1.1 become's 1, and 1.2 becomes 2.
I was trying to ask the community at large if anyone knows of any pro's or con's to either method that would lead you down a specific path beyond personal preference.
Regards,
Kyle
If so, ya that actually helps. takes a couple clicks out of my work flow and i am all about that.
Yes, that is exactly it. What you could have done was make a promoted assembly of the bracket with the fasteners and whatever else was required and then use that promote assembly to do a pattern or something along those lines.
The way you did it works too, it's just a lot more ''intensive'' for SolidWorks to work with since it has so many more mates to solve.
So i ended up not doing it in a pretty way but it was a lot easier than copying each subassembly and then manually doing 3 mates, ie clicking on two faces and than coincident mates.
Copy with mates got the job done a lot faster. first time using it and learned a new thing today.