Welcome to the Onshape forum! Ask questions and join in the discussions about everything Onshape.
First time visiting? Here are some places to start:- Looking for a certain topic? Check out the categories filter or use Search (upper right).
- Need support? Ask a question to our Community Support category.
- Please submit support tickets for bugs but you can request improvements in the Product Feedback category.
- Be respectful, on topic and if you see a problem, Flag it.
If you would like to contact our Community Manager personally, feel free to send a private message or an email.
purpose of setting the origin or chosing a new defined mate in a context design?
kees_bijker
Member Posts: 148 ✭✭
So I use "in context design" a lot and it is a very powerful way to design something that works together with other parts.
I have noticed that nothing much changes when you choose the origin or when you make a self defined mate as origin for your in context design. I followed the "in context design" course till about 50% now, and I still am no wiser as to why you have to chose the origin opposed to it simply being the origin of the assembly?
I tried both and I cannot find any advantage of chosing your own mate, so please let somebody explain to me what is the difference and for what is it used normally?
I am sure I am missing something which could be really useful, so I want to add that to my tool box if I can.
Thanks in advance.
Best Answers
-
eric_pesty
Member Posts: 2,127 PRO
The main reason why you would want to use a specific mate connector is that the origin of the in context part will follow that mate connector, and the front/right/top orientation of the in-context part can be set that way instead of following the assembly origin and orientation.
0 -
MichaelPascoe
Member Posts: 2,243 PRO
The advantage of selecting a mate connector would be when you want the part studio's planes and origin to align with the center of a specific part. For example, maybe your creating a robotic arm and you have a cylinder that isn't at the assemblies origin. If you use a mate connector as the origin reference, your part studio can start with it's planes and origin correctly placed on that cylinders axis. This way you can immediately start using those planes to create sketches, instead of having to create another mate connector to reference the cylinder again.
Learn more about the Gospel of Christ ( Here )
CADSharp - We make custom features and integrated Onshape apps! Learn How to FeatureScript Here 🔴0 -
eric_pesty
Member Posts: 2,127 PRO
What I meant was that the new part's coordinate system would match (better than follow) the mate connector.
This helpful if you need to create an in-context part that is not "aligned" with the assembly x,y,z axes.If you create the mate connector in the assembly and use for the in-context part, then you can create a mate connector at the origin of the part and mate that to the assembly in-context mate connector.
Then your part will follow that assembly mate connector. Note that context don't update automatically, you have to intentionally "update context" if you move the mate connector in the your assembly for the part geometry to update.
1
Answers
The main reason why you would want to use a specific mate connector is that the origin of the in context part will follow that mate connector, and the front/right/top orientation of the in-context part can be set that way instead of following the assembly origin and orientation.
The advantage of selecting a mate connector would be when you want the part studio's planes and origin to align with the center of a specific part. For example, maybe your creating a robotic arm and you have a cylinder that isn't at the assemblies origin. If you use a mate connector as the origin reference, your part studio can start with it's planes and origin correctly placed on that cylinders axis. This way you can immediately start using those planes to create sketches, instead of having to create another mate connector to reference the cylinder again.
Learn more about the Gospel of Christ ( Here )
CADSharp - We make custom features and integrated Onshape apps! Learn How to FeatureScript Here 🔴
Thank you eric_pesty and MichaelPascoe, Very clear and to the point.
I will have to try it from this point of view once and see what I can get done better and faster this way.
Kind regards,
Kees
As illustrated above, when moving the mate connector specified as the origin of the new "in context part", the part stays in place. Saying that "it will follow the mate connector" is not what I observe…
A second effect of moving (or any change to) the MC is that the part "looses" its references to the MC and fall back to the default assembly origin.
@bernard_lucas
Your part 2 is not connected to part 1. You created a new parts studio on a mate connecter that had certain coordinates at that time. Onshape will continue to use those coordinates unless you have a true-in-context loop and force an update.
Now, should onshape move the coordinates of the parts studio based on Part 1 is an entirely different and very controversial matter for which you could submit an improvement request if you feel it should be the default behavior.
Thank you, @wayne_sauder, for your response.
Since this discussion centers on the specific scenario of choosing between an assembly or an MC reference system, I wanted to share my thoughts on @eric_pesty's remark stating that "the origin of the in-context part will follow that mate connector."
Regarding your comment, "Your part 2 is not connected to part 1," I agree. If I wish to connect the parts, I can simply use a mate, so this isn't the issue.
Now, if I understand you correctly, you're suggesting that the situation changes when a context is established (for part 2) and updating that context will have an effect. You appear to imply that the effect would make part 2 follow the initial MC—but that’s not the case. For clarity, I initially reduced the issue to its simplest form. Here’s the "context" version of the same example. After updating the context, the reference system remained unaffected, and, as before, "part 2 did not follow the MC."
The primary question remains: why should one select an MC as a reference? Shouldn't it be explicitly stated that selecting an MC as the reference system is a "one-shot" choice, meaning it won't adapt to subsequent updates made to that MC? While this behavior isn't inherently an issue, it does challenge our natural expectations.
@bernard_lucas
I understand what you are saying, and no, I was not trying to imply that the in-context workflow would move things the way you wish it would. I was simply trying to say a mate between the parts takes care of this issue.
Try this: add a mate connector to a parts studio. Use that mate to create a new parts studio, make a part, and insert it into the assembly. Now move the mate connect in some way, rotate it as well, then select your part and edit in-context. (you do not need an in-context reference, but your part must be mated in the assembly, not just free-floating). Notice that the coordinate system follows the mate. I think this is what @eric_pesty was referring to when he commented that the origin will follow the mate.
Keep in mind that there are some advantages to creating mate connectors over using the one available on the parts.
Your primary question remains.
Thank you again @wayne_sauder for your reply. Maybe I did not express my concern properly.
My question was not whether selecting an MC as the origin should behave in a specific way or not.
What I am trying to understand are the actual implications of this option. I don't have expectations.
I am simply looking for clarity on what this option truly does.
Would you agree —as an official Onshape PRO reference— on this crucial point: selecting a mate connector (MC) as the origin of a new part does not result in that part "following" the MC?
Thank you so much for your time and attention.
Best,
Bernard
According to me, and I am in no way an expert, is the chosing of the mc in no way relevant for the cad or the part or the designing at all. It choses its plane and point of reference for when you export or wish to make an assembly so that the part after insertion or export shows the same orientation as the assembly you want to use it for.
Try this: you start an in context part studio for something and you chose the origin of this part studio as the in context mc. Your part when inserted in this assembly will automatically be oriented correctly.
Now do the same but chose a mc that is not orientated the same direction, you may have to produce one specially for this purpose but just do it. Now when you insert this new in context part in the assembly, it will follow the mc you chose. So if in original assembly front was the right plane of your chosen mc for the in context part, after inserting it projects the part initially with its own front to the front and not alligned with the front of the assembly.
Same when you export a part for printing for example. Normally the base of the part is what is down in your cad environment, but if you rotate a part inside your assembly to match the assemblies orientation, this part will appear rotated after export.
Try something else: you design a machine with a 30 degree top surface. You make your basic parts in a part studio all with the origin the same way, because they are in the same part studio. Now make an assembly of these parts, they are all orientated in the same direction. Now create an in context part studio and chose the origin of the assembly but you allign your in context part along the 30 degree worktop of the machine.
Now it will be inserted correctly for this assembly, because it was created in the same environment, but now export this part for printing and you will notice that it does not sit flat on the build plate. Also, if you go back into the in context part studio to correct this, you do a transform of 30 degrees, and the part now sits flat on your build plate after export. But if you now go back to your assembly you have broken it. This part, and all the ones you mated with it, will be rotated by the same 30 degrees and your mc list will have some red flags in it. This is what it does, the “follow the mate connector origin” does not mean anything for the design or the parts as such. It only means that it follows its origin orientation during assembly and export. Also it does the same when you generate a drawing of this part. The origin of the drawing is like the part studio it was formed from but if the part pokes up with 30 degrees, it will show up in the drawing at 30 degrees.
What I meant was that the new part's coordinate system would match (better than follow) the mate connector.
This helpful if you need to create an in-context part that is not "aligned" with the assembly x,y,z axes.
If you create the mate connector in the assembly and use for the in-context part, then you can create a mate connector at the origin of the part and mate that to the assembly in-context mate connector.
Then your part will follow that assembly mate connector. Note that context don't update automatically, you have to intentionally "update context" if you move the mate connector in the your assembly for the part geometry to update.
That is how i understood it but I think the word 'follow' made people think it would litterally follow and when it changes it would change with it.