How would you mate this to get it to go in and out the slot and rotate in the circle I used limit distance to get it to go up to the slot and back out. If there isn't a way how can I mate it just to rotate around the circle and make it stay in the center.
Bigl Cadking wrote:
you can download it here it is the
Car And Caravan Laser cut
Leland Pike | CAD Models | GrabCAD
Many respondents won't download files outside of the forum, so you're limiting your replies by doing so.
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In the upper right of your original post (OP), select edit and attach the files there.
Kevin
Here is the assebly and all the parts in the tset rar file
I have only Windows OS on my clean SWX machine (I don’t own a rar extractor).
here is each part
And you call yourself Big Cadking! You cannot do it in a single configuration. Best you can do is the limit mate in one configuration that also restricts rotation. Other configuration would suppress the limit mate and rotation prevention mate and unsuppress a coincident mate between an axis centered in the pin and the axis of the circular hole.
I spoke too soon. Got something that works assuming the slot is wider than the pin. You do have to be careful and move real slow and deliberate. If it goes haywire, suppress the Pathmate4 and reposition until suppressed mate is solvable again and un-suppress.
I would model CC1-1.sldprt with symmetry about the Origin. (This pays dividends in setting assembly DoF.)
I would fully constrain the sketch without -
duplicate dimensions
diameter overtop equivalent radius
dimension that cannot be measured on the shop floor (or even in inspection lab).
Dimensions can be reduced (and part editing made easier) by using obvious geometry constraints (relations).
In the real world we cannot manufacture perfect parts.
There should be clearance between the "peg" at MMC and the "slot" at LMC.
(I guess if the material is soft wood we could force interference compression of the material.)
Do have SolidWorks version with advanced motion analysis, or are you merely trying to do an animation?
I have not downloaded your files so I don't know if you have already tried this or not but if you added a center line to the upright 'tab' and align that geometry with the center line of the hole then it might work. I don't know about the translation portion though.
Hi,
I think that the old „limit trick“ will work for you:
Create a sketch with only a point in the woving part on the contact surface. It should be positioned right in the rotation axis.
Create a 2nd sketch int the part with the slot, also on the contact face. Draw a linear spline from the middle of the bore along the slot. As long as the part should/could move.
Now add 2 constraints. 1st is the contact between the two faces (coincident) and the 2nd between the point and the spline. From now on the point can only move along the „path“ and is able to rotate...
Sry, but I‘ve got no SWX on my iPad...
Heiko Sohnholz wrote:
Hi,
I think that the old „limit trick“ will work for you:
Create a sketch with only a point in the woving part on the contact surface. It should be positioned right in the rotation axis.
Create a 2nd sketch int the part with the slot, also on the contact face. Draw a linear spline from the middle of the bore along the slot. As long as the part should/could move.
Now add 2 constraints. 1st is the contact between the two faces (coincident) and the 2nd between the point and the spline. From now on the point can only move along the „path“ and is able to rotate...
Sry, but I‘ve got no SWX on my iPad...
I seem to remember a recent challenge to restrain an item in an arbitrary box - this sounds like a similar situation/solution.
The issue wit this is that the coincident between the two faces will prevent it from rotating.
I've donwloaded your files, followed my own advice ... what should I say ... works like a charm!
Please try again.
Another attempt could be using "Move Component" and check the option "Physical Dynamics". But you should makre the slot a little bit wider first...
Attach assembly here.