What is the preferred method of positioning/locating holes in two different parts so they line up when mated? Imagine I am creating box and a top to said box. The side edges need to align...and the screw holes need to align.
What is the preferred method of positioning/locating holes in two different parts so they line up when mated? Imagine I am creating box and a top to said box. The side edges need to align...and the screw holes need to align.
Hi Kingsley,
In a part or assembly go to View and turn on the Temporary axes.
This will add hole centre lines, then when mating just select the two axes lines and holes will align.
Thanks
Mark (SolidWorks 2015 sp4)
Kingsley,
If you have two fixing holes in each part then you just need a Concentric mate for each hole & a Coincident mate for the two surfaces that sit against each other when the lid is fitted.
Maybe I wasn't clear. I understand how to mate parts. What I don't understand is how to locate the holes in individual parts when I am making them so that all the holes (and other features like sides) line up when I go to mate them. It would be easy if I were making two cylindrical parts that needed to screw together with one screw by putting a similar screw hole in each part at the center of each cylinder -- got that. But what happens with more complex parts? Staying with our two cylindrical parts, assuming we want the parts themselves to align on the cylindrical axis how would we locate TWO screw holes in each parts such that when they are assembled the holes would align. (If they did not align and we asked for concentric mates on both screw holes we'd be over constrained and the mate would not work -- in addition to the part not looking right).
Don't dimension circle in one sketch. In sketch, constrain center to center of mating hole. (Parts are mated already at assembly).
I use a Sketch Part where I have over 90% of all my sketches and planes - I drop this part into an assembly and when I insert a new component I would select the sketch with the hole and convert the entities then when I add the second part and that needs the same hole reference then I would pick the same hole sketch and convert the entities, now these two parts will align perfectly and if I change my hole size or location within the sketch part both follow......
Or you could use the same construction sketch for the parts, so the sides align. Are you using the Hole Wizard? If so, copy the position sketch from first part to the second. Redefine relations appropriately.
Hi Kingsley,
As you can see form the reply's as is often the case there are multiple ways to do this.
Having read through these I would agree with Glenn, the easiest way would be to bring blank plates into an assembly mate then add the holes and propagate to the part.
This is how I would do this, but that is just my preferred way. Others have there own way of doing this.
Thanks
Mark
As you say there are numerous ways of doing this. I like this the best from my point of view. Many of the other methods would be useful too. Thank you.
Edit one part In-Context of the assembly.
In-Context is a core function of Solidworks parametric modeling.
Search Solidworks help for Editing a Part in an Assembly
Assemblies > Top-Down Design > Editing a Part in an Assembly
With this technique you can have the holes on lid follow the holes on box or vice versa.
Hello,
In the assembly with the two parts positioned as required, you can add a Hole Series (under Assembly Features).
You can also add a hole in one part, mate the assembly and then use the part's hole to put the hole in the second part using Hole Series.
Cheers,
Kevin
For one more idea, you could create both Parts without any holes. Bring them into the Assembly and mate them as you want. Then create the holes with an Assembly feature (Hole Wizard, Extruded Cut, etc.). Have the feature propagate to both Parts.
If you want the holes to always be concentric on both parts, then use in-context edits (and by virtue also external references) or a assembly feature like others have mentioned.
But I'm going to throw another method in the mix. If the part your making might be used in a lot of other assemblies, or future holes and parts might be added on, external references might not be the best solution as you can end up with circular references or mysterious moving holes if you don't pay attention.
One way is to create the external reference and features, break the link, go back to the sketch, and then pull locating dimensions just like you normally would. You can also create driven(reference) dimensions before you break the link, in case your worried about accidentally moving it or the dimensions not being the same, and then just make them driving after breaking the link.
If you have a good understanding and usage of planes, then you should be able to just pull dimensions off your mid-planes and edges and get them to line up normally.
If you don't like external references, and maybe are not so good with planes, or just want to be difficult and do it manually, then do the following:
- Mate parts in assembly accordingly
- Pick one part, insert a hole exactly where you want it
- On the second part, put a hole in the general vicinity of where it should line up.
- Go back to the assembly, use the measure tool to get the center to center distance between the holes, then adjust the second hole position accordingly.
Note that if you have varying amounts of decimal places in each part or on your measure tool, you can build up a small, small difference as SW always uses 8 places, and then rounds it to your document/template settings. This generally only occurs when you don't type in an exact/rational number for a dimension or drag components to the distance you desire after dimensioning. When this happens you can end with parts with dimensions that you see as 36.125", but really might be 36.12501648". Being off on a hole by 0.0001 will have zero manufacturing impact for most people, but depending on how you mate components, SW might throw an error when trying to use concentric mates as it always resolves mates and dimensions using 8 decimal places. I see this a lot with legacy sheet metal and AutoCad imports, when designers were too lazy to redraw them natively in SW. Also happens with bad rounding, like 7/32 being just entered as .218 vs .21875(.219) or 9/64 being .140 vs .140625(.141) when using 3 decimal places. Just this week, my punch guy raised a fit about double punching because whatever ancient software we've been using has been set to .21800000 for the punch and it doesn't like seeing .218750000, so it double punches. -.-
But anyway, those are your options. Plenty of ways to different ways to get it done.
To add another 2 cents worth...a note about mates (and expand on Andrew Deboer's point).
If two parts have a hole pattern that drives the rest of the mating parts, then I use the holes to mate (concentric). To fix the part I use parallel mates rather than coincidence mates. This allows for any minutia of misalignment and also reduces over definition of mates. If the two parts are assembled by a feature (rib/slot combo or such) then I use that as the primary mate. It is similar to dimensioning a part for design intent. Maybe that is obvious...but I thought I'd share it anyway.
Hi Kingsley,
As you can see form the reply's as is often the case there are multiple ways to do this.
Having read through these I would agree with Glenn, the easiest way would be to bring blank plates into an assembly mate then add the holes and propagate to the part.
This is how I would do this, but that is just my preferred way. Others have there own way of doing this.
Thanks
Mark