I'm having trouble with mate,
I use the 3d interconnect so that i do not need to convert igs to solidworks native files, when i use mate it won't allow me to select the second face is it a bug or not im using solidworks 2018 sp3
I'm having trouble with mate,
I use the 3d interconnect so that i do not need to convert igs to solidworks native files, when i use mate it won't allow me to select the second face is it a bug or not im using solidworks 2018 sp3
Can you upload your models here so other can try and help you out
Hi christian,
I attached the files but i do not know why the files was zip i upload them as raw file which is not zip
The forum uploader will automatically zip any file which is uploaded in my experience.
Xy,
I don't think your parts you are trying to mate have any planar faces or edges. If you look at the example below the only option I get for the two edges is tangent, indicating one of them is a curve. I also get the same option if I select two faces. If I select two vertices I get the option of coincident mate.
The mate you did manage to add was using the plane of one of the parts.
The face should be planar since all the model was previusly created from sw2007 version the original sw file was lost we only have the igs so i just use 3d interconnect so that i will not re create the entire cross flow turbine. Does other has the same problem when using 3d interconnect
If you don't want to change the feat, you can add/use the ref. plane for mating
If you don`t want to recognize geometry to make it precise, you can use vertex to surface or vertex to edge matings.
Igor Fomenko wrote:
If you don`t want to recognize geometry to make it precise, you can use vertex to surface or vertex to edge matings.
You can also use edges to create planes for mating...same thinking.
Cheers,
Kevin
Recently, I had similar problem - I was not able to select planar faces from imported *STEP. Solution was to turn 3DInterconnect off.
Ill try that when i get back to work
Xy,,, This is an interesting dilemma. Certainly is not the intended behavior for 3d Interconnect. I can't be sure if this has been an issue in previous service packs or is something that SP3 broke. I can't remember having the problem with earlier service packs but unfortunately don't have one to test it with. Perhaps someone can do this for us.
I did find that if you dissolve the parts in the assembly then open them you cannot put a sketch or plane on any surface. BTW the parts become virtual in the assembly and still appear to be linked to the original iges. In order to make the surfaces "usable" I deleted a face on each part (with the "Fill" option). After that all the faces become usable for sketching, mating, or whatever.
There is definitely something going on and I'm guessing it is with the SP.
I did check in with the good folks at GoEngineer (my VAR) and brought this to their attention. Like all of us they were taken aback with this behavior. They were very grateful to you for bringing this to their attention.
Until this gets resolved I suppose you can come up with a workaround of your own or use some helpful hint from others.
Or...... Just don't use 3d interconnect.
Hi Dennis,
I brought this to the attention of my SOLIDWORKS team here at GoEngineer and we deemed this a high level issue with 3D Interconnect. I have submitted Service Request# 1-17987293571.
Thanks Dennis,
Indeed i try the sp2 and it has the same issue unfortunately i don't have extra computer and the sp1 to try it. Thanks everyone after incorporating the suggestion of everyone i finished my work just in time here is what it look like.
I log in, in the solidworks customer portal but i cannot find where i can vote for the SR, (my subscription is active)
I think that takes a couple of days to get into the system.. I talked to my VAR on Friday. I will ask them about that on Monday.
Ok thanks
An update to this.. The SR is now an SPR.. SPR# 1049584 and can be voted on. Apparently the issue is with the IGES importer (non prismatic topology). Until the issue is resolved it is suggested to use STEP files as a workaround (if possible).
Thanks Dennis
Hello All,
I believe I have a fix for this. I was having the same issue where an IGES file would not allow me to add mates within the assembly.
Browse to open your file within Solid works. Click it once ( do not open) and select "Options". Change the top drop down menu from *IGES to "General".
This will allow you to add mates like a normal assembly file.
Cheers!
Xy,,, This is an interesting dilemma. Certainly is not the intended behavior for 3d Interconnect. I can't be sure if this has been an issue in previous service packs or is something that SP3 broke. I can't remember having the problem with earlier service packs but unfortunately don't have one to test it with. Perhaps someone can do this for us.
I did find that if you dissolve the parts in the assembly then open them you cannot put a sketch or plane on any surface. BTW the parts become virtual in the assembly and still appear to be linked to the original iges. In order to make the surfaces "usable" I deleted a face on each part (with the "Fill" option). After that all the faces become usable for sketching, mating, or whatever.
There is definitely something going on and I'm guessing it is with the SP.
I did check in with the good folks at GoEngineer (my VAR) and brought this to their attention. Like all of us they were taken aback with this behavior. They were very grateful to you for bringing this to their attention.
Until this gets resolved I suppose you can come up with a workaround of your own or use some helpful hint from others.
Or...... Just don't use 3d interconnect.
Hi Dennis,
I brought this to the attention of my SOLIDWORKS team here at GoEngineer and we deemed this a high level issue with 3D Interconnect. I have submitted Service Request# 1-17987293571.