New to Alibre, Some Qs

[simonb65]

I was told once that "Not responding" means that it's too busy to respond to your input. Kind of like "don't bother me now I'm working".

It happens when an application is tied up in a tight loop 'doing stuff' and ignoring Windows. Each application is run on Windows as a time sliced task with a message queue to and from the OS. If that message queue isn't being serviced by the application, it gets flagged as 'Not Responding'. That isn't good practice. Even in tight loops that take time, the application should periodically service the Windows queue, just in case windows want to 'ask' the application to close, minimise, maximise, etc. In short, a well written application should never become unresponsive to the OS!

From Google ...

"An application gets events from a queue provided by Windows. If the application does not poll the event queue for a while (5 seconds), such as doing a long calculation for example, then Windows assumes that the application is hung and alerts the user."

For example, this pseudo code will cause the application to become unresponsive ...

Do the next bit inside the curly braces 10,000,000 times as we process all the geometric data (it may take a while!)
{
Do something like a calculation on the data here
}

This pseudo code will allow the application to be responsive ...

Do this next bit inside the curly braces 10,000,000 times as we process all the geometric data (it may take a while!)
{
Do something like a calculation on the data here

Check and process any messages from the OS <---- This also ensures the user can still do stuff like drag the application window around and keeps the OS happy.
}

 

[kcoffield]

Me again. I did a little more with this intake manifold flange. There are two sets of mounting bosses at different angles. I generated planes (at angles through axis) to build the boss profiles at the correct angles. The first set seemed to work fine (sketch 5 on plane 18). I can't get the second set (sketch 6 on Plane 20) to extrude but no errors reported as to why. Any ideas why?

All the points were there to locate the center of the port windows and mounting boss locations. The points now say they aren't associated with known geometry. Not sure how/why that happened, but I can still select them.

If I can get the bosses extruded I figured I'd trim away the unwanted portions, do some filleting and unite the pieces. I'm not very good at reading everything the design history is telling me.......but trying.

Any help is much appreciated.

Best,
Kelly

 

[Ken226]

Me again. I did a little more with this intake manifold flange. There are two sets of mounting bosses at different angles. I generated planes (at angles through axis) to build the boss profiles at the correct angles. The first set seemed to work fine (sketch 5 on plane 18). I can't get the second set (sketch 6 on Plane 20) to extrude but no errors reported as to why. Any ideas why?

All the points were there to locate the center of the port windows and mounting boss locations. The points now say they aren't associated with known geometry. Not sure how/why that happened, but I can still select them.

If I can get the bosses extruded I figured I'd trim away the unwanted portions, do some filleting and unite the pieces. I'm not very good at reading everything the design history is telling me.......but trying.

Any help is much appreciated.

Best,
Kelly

Im not sure why it's not extruding for you. I un-suppressed the sketch and clicked extrude, and it extruded.

Which direction and distance are you extruding to?




In your sketch, try this:

Rather than inserting a bunch of points and using those as references, dimension one of your port loops horizontal and vertical sketch figures relative to the default X and Y axes. (I created my first loop on the origin, which causes inferred constraints which lock down its position). From that point, you can use the constraints and dimensions to lock everything else down relative to those. Ideally, you'd like to have your sketch constrained so that future modifications will be much easier.

I don't fully constrain all of my sketches, but stuff that is likely to need changes later get more attention to constraints. Dimensioning sketch figures relative to the stock axes should define their position in space, whereas dimensioning the length of a line, radius of an arc, etc should define its magnitude. An ideal sketch would be all black, with each figure having its magnitude and position defined.

Of course, that is also time consuming, so ya kinda pick and choose when/where to do it.

 

[HaroldL]

Me again. I did a little more with this intake manifold flange. There are two sets of mounting bosses at different angles. I generated planes (at angles through axis) to build the boss profiles at the correct angles. The first set seemed to work fine (sketch 5 on plane 18). I can't get the second set (sketch 6 on Plane 20) to extrude but no errors reported as to why. Any ideas why?

All the points were there to locate the center of the port windows and mounting boss locations. The points now say they aren't associated with known geometry. Not sure how/why that happened, but I can still select them.

If I can get the bosses extruded I figured I'd trim away the unwanted portions, do some filleting and unite the pieces. I'm not very good at reading everything the design history is telling me.......but trying.

Any help is much appreciated.

Best,
Kelly

Like Ken, I was able to extrude sketch<6> without any problem. The only reason I can think that it may not have worked for you it that you had an illegal Type set in the extrude dialog. It will extrude with all except "To Next". If you try the extrude and it shows an error check its status, it may a have this "9007: Disjoint loops not supported for To Next extrusions" in the status message if To Next was selected. Otherwise it's a mystery.

As for all the Point errors. If you RMB click on them and select Status from the popup menu they all have the same "The source of this geometry is not found" status. Somehow, it seems,the nodes that were used to locate the points have gone missing and need to be replaced.

Hint: One thing you might try is to create an offset planes, from planes 18 and 20, by the distance you want the ports to extend. Create your sketches on those offset planes then extrude "to geometry" and select a face on the flange as the target. That way you won't have so much trimming to do to get your final shape. And for trimming try out the Remove Face tool, that way you won't have to set up sketches and extrusions to remove the extra bits you don't want in the model.

Hint: So you don't end up with a complex and complicated sketch, sketch and create on feature then use Feature Pattern to create the rest of the features. That way if you need to modify the the feature you only have one simple sketch to change and all the remaining features will update accordingly.

 

[kcoffield]

Im not sure why it's not extruding for you. I un-suppressed the sketch and clicked extrude, and it extruded

Doh! It was simply because sketch 6 was (inadvertently) suppressed. I also had the angle of the plane for one of the sets of bosses which I corrected. The intake flange is now essentially complete except trimming away the excess boss geometry and maybe some filleting.

Rather than inserting a bunch of points and using those as references, dimension one of your port loops horizontal and vertical sketch figures relative to the default X and Y axes. (I created my first loop on the origin, which causes inferred constraints which lock down its position). From that point, you can use the constraints and dimensions to lock everything else down relative to those. Ideally, you'd like to have your sketch constrained so that future modifications will be much easier.

The blueprints I'm working from are from the intake face of the cylinder head, so all the positions of features translate to the backside of the intake flange. The primary datum on those drawings is actually a reference 3-space point on the engine block which doesn't translate very sensibly in many respects to the intake manifold, but I have used them to avoid a lot of dimensional translation......though suboptimal.

An ideal sketch would be all black, with each figure having its magnitude and position defined.

I took note of fully defining sketches from the various tutorials though struggle a bit to do so, and when I do, I seem to run into other problems downstream caused by the constrained objects......but I'll keep at it.

Hint: One thing you might try is to create an offset planes, from planes 18 and 20, by the distance you want the ports to extend. Create your sketches on those offset planes then extrude "to geometry" and select a face on the flange as the target. That way you won't have so much trimming to do to get your final shape. And for trimming try out the Remove Face tool, that way you won't have to set up sketches and extrusions to remove the extra bits you don't want in the model.

Thanks for that. I updated the file attached below (updated rev 5) but have not trimmed off the excess bosses. I can certainly see how it be better to just avoid it altogether with the extrude to geometry suggestion. Removing the bits in the scalloped areas looks tricky. Where is Remove Face Tool? I have design Pro. Is that an Expert feature?

As for all the Point errors. If you RMB click on them and select Status from the popup menu they all have the same "The source of this geometry is not found" status. Somehow, it seems,the nodes that were used to locate the points have gone missing and need to be replaced.

Yes I surmised such but not sure how the nodes disappeared unless I was dragging the feature/sketches around in the design history.

Hint: So you don't end up with a complex and complicated sketch, sketch and create on feature then use Feature Pattern to create the rest of the features. That way if you need to modify the the feature you only have one simple sketch to change and all the remaining features will update accordingly.

I will definitely give this a go on my next revision. The Alibre documentation for Pattern says "Only dimples, sheet metal cuts, and holes should be patterned." but I noticed in the tubular header example that Ken226 posted that doesn't seem to be the case. I wasn't success using it in my first attempt. It wants to copy the feature to a liner grid, and although the two sets of bosses are linear, they are not equally spaced, so I would have to apply a pattern for the second, third, and fourth boss in each set....is that correct? The Port windows are equally spaced. It would be very nice to be able to change the size of the port window and face of the bosses and have the model update, so I'll have to work on this.

I'm sure I'll build refine this part a few more times as it is my first part and learning exercise.

Thanks for your help fellas. I'm making some progress.

Best,
Kelly

 

[HaroldL]

Where is Remove Face Tool? I have design Pro. Is that an Expert feature?

The Help manual indicates that Remove Face is available in the Pro Model tab.




I would clean up the extrusion as shown. Assuming the bits indicated are not needed on the model.

The Alibre documentation for Pattern says "Only dimples, sheet metal cuts, and holes should be patterned." but I noticed in the tubular header example that Ken226 posted that doesn't seem to be the case. I wasn't success using it in my first attempt. It wants to copy the feature to a liner grid, and although the two sets of bosses are linear, they are not equally spaced, so I would have to apply a pattern for the second, third, and fourth boss in each set....is that correct? The Port windows are equally spaced. It would be very nice to be able to change the size of the port window and face of the bosses and have the model update, so I'll have to work on this.

It looks like that part of the Help manual needs to be rewritten or at least clarified. It sounds like it is focused on sheet metal features and should be in the Sheet Metal section of the manual.
As it further indicates, you should be able to pattern extrusions, both Cut and Boss, as well as other solid modeling features. As for features that are not equally spaced you would need to create them individually. I think it has been submitted as a feature enhancement to allow the Linear Pattern tool to accept unequal spacing of features. Don't know if it has been evaluated by Alibre Dev yet.

 

[kcoffield]

The Help manual indicates that Remove Face is available in the Pro Model tab.

It was labeled differently, and I just hadn't expanded the drop-down menu. Thank you.

I would clean up the extrusion as shown.

I was able to use that to clean up the model. TY

As it further indicates, you should be able to pattern extrusions, both Cut and Boss, as well as other solid modeling features.

I think I'll try another iteration of this part using these associated build features to make it more editable/parametric. Should be a good learning exercise.

Attached below is a picture of the completed part filleted..........except for one stubborn boss second from the end on the right which returns errors.

Thanks for your helpful suggestions. Much appreciated.

Best,
Kelly