* Q1: How I can increase the size of the arrow head. So that the green arrows are the same size as the (1) red arrow. Should be simple but I've tried everything.
A1: Arrowhead size and color for balloons and most other things can be changed in AMOPTIONS (Annotate->Annotation Options), then double clicking on Leader in the list.
(yes and in MDT4, AmOptions did not lead me to be able to change arrow size. I double left clicked on the leader itself onscreen (AMPOWEREDIT) and up jumped the Properties dialog box and I changed the arrow from 2.5 to up to 9.1 but over at 9.2 on the arrow disappeared. Similarly the arrow on the Section A-A line. It would go up from 2.5 to 3.1 then disappeared from 3.2 on. Note AMPOWEREDIT gives the same result as PROPERTIES. -aj)
Q2: Secondly, how do I change the balloon circle colour ONLY.
A2: Again, AmOptions select Drawing tab, double click on Layer/Objects select Objects tab, and find 'Balloon Geometry' (Hint you can click on Descriptions to get it to sort the Descriptions by name). Then just pick a new color for it.
Q3: Thirdly, how do I increase the arrowhead size of the hole note?
A3: See A1.
Q: Fourthly, the why doesn't the hole note follow the dimstyles settings. How do I get this useless command amnote to follow the dimstyles for text size, height, font blah blah blah.
A: Look up the DIMSTYLELIN function both in help and by searching this newsgroup. There has been lots discussed about it. The software will do most everything you need it to, you just have to learn how to use it!
See Link1 Link2
* All of Mechanical Desktop requires acme.arx
* Top part in browser is grounded part. Any other part contrained to it will re-orientate to it. Either reorientate the grounded part or shift and drag another part up to the top position in the browser. Note heard somewhere about making a dummy first part to allow cetain actions (think todo with toolbodies and dies). Also how about a extra cube part for manipulating blob shaped things can be rotated accurately?)
* E Transmit to take a folder somewhere else to work on it or look at it ie File->E Transmit. Send every thing to a special folder for the purpose then zip the contents for that folder up to send as an attachment to an email or put somewhere to be accessed for downloading via ftp or off the http.
* When you create a hole note for a counterbored hole, it will place the depth symbol even though the hole is going thru. So it in the Hole Note editor (delete depth/symbol) before placing it. Alturnatively, if you do a lot of thru counterbored holes, create a teplate and select it when you are adding hole notes for that type of hole.
* CMM Coordinate Measuring Machine.
* Rename external files Douglas Weekly May/13/03
* It appears that the 2D constrain bug (lose project constraints after appending a sketch) still exists (in MDT6/7).
* SETVAR, then ? Enter, then * Enter .. to see all the system variables and their settings.
* Use Scenes to control which assembly parts appear in a layout and suppress sectioning of shafts (and 'independant' webs).
Making a Layout directly of a sub-assembly model will give you all the parts wether you like it or not. One advantage of doing a Scene is you can turn off visability of parts you don't want and make a Layout consisting only of the parts left visable. Another advantage is you can use an Explode Factor and Trail if desirable and a real biggie is you can suppress the sectioning of a pin or shaft that lies on your section line or plane. If you make the web as an individual part and constrain it in place the in a Scene you can suppress the sectioning of that part. If you do an AmCombine treating the web as a tool body the web/toolbody 'feature' identifiable in the model browser tree is doe not occur in the Scene browser tree so you cannot do a section suppress that way.
* Inventor has parametric surfacing but cannot bring in surfaces and repair them. MDT can.
For new projects you should be able to create any surface you need in Inventor with the advantage that they are parametric. However it is still easier to edit poor surfaces translated from other programs in MDT (such as customer iges files of 3D surfaced parts). I am not aware that Inventor 7 includes any surface editing tools for repairing surfaces not created in Inventor. I believe the whole philosphy is that surfaces are infinitely thin reference geometry, not representations of real-world solids.
* Not good practice to MOVE a sketch. Fully constrain (including dimensions) the sketch. Erase the fixed contstraint. Use a grip to 'stretch' to new location. The sketch will not actually stretch as it is dimensionaly constrained. Add a fixed constraint in new location.
* Q: In MDT how you can put a thin rubber coating on a part by
A: In the assembly catalog right click on the part & copy definition. Then shell the part to the outside by the coating thickness. Note that individual surfaces may have their thickness modified.
* Why some shops won't use table driven parts.
Consider a part with just two table driven versions. In the assembly drawing when you change the second instance to version 2, the first instance also changes. Only answer is to have one instance and copy the definition, from AMCATALOG, of the first part. I understand Pro-E is the only MCAD program that has this functionality (it's not in Inventor as at IV7 although it is asserted that iParts 'for the most part' give you that functionality).
The method above works but you are now creating a non-linked version of theexternal part within your assembly file - this works fine for a number of industries - especially those that have part numbers linked to a Job.
In my work, I have to be able to maintain all part numbers used. If you make a change to a part it has to show up in the documentation for every assembly where it is used because that part will do the same thing out in
the shop.
I use table driven parts to create my part families during product development but before I go to production I have to create each version of the part as a stand-alone file and create the assembly drawings using these
stand-alone parts. For me, anything less than a linked file with revision control on each version won't work.
* js: Is it possible to move an ortho section view to a different layout than the base view?
aj: You can RMB on the original layout in the browser and copy the layout (to say 'layout 2' and then delete the base view in layout 2 - even though the base view is gone, the section will still update to changes (tweaks) in a scene (assuming this is a section of a scene, not a single part).
(Actually in MDT4 did not appear to have a copy option so for the exercise I did a (in browser) RMB on Base View -> Move then (ignoring elastic line from center of base view to the cursor tip) enter L (for Layout) then Layout2. After LClicking to indicate an insertion point, the dimensions, centerlines and sectioning moved along with the browser tree into Layout2 but there was no part outline! Using RMB->Move on the Ortho view gave the elastic connection to the cursor tip but no option was provided at the command line to move to a different layout All you could do was move along a perpendicular line to the Base view within Layout. Perhaps there is a definite Copy option in MDT6. -aj)
js: If you delete the base view the section arrows still show up. I guess I can move them to a non-visible layer. And there we go again with the scene stuff. I'll need to start using scenes for every drawing not just assemblies.
aj: Actually, when I tried this I just erased the arrows - it didn't seem to hurt the section view, but didn't check if they (the arrows) would re-appear during an update to the layout
js: When I delete the arrows it also deletes the 'section a-a' label in the section view. Simple to re-create but then the text isn't attached to the view.
kt enters: Then run AMANNOTE, select the new ones you just created, and attach them to the view. now they'll move with the view.
db enters: After you rebuild it use the amanote command to attach your label to the drawing view.
* Inserting an MCAD drawing in to Word.
(.in the following you have to consider some or all of the following: pre-sizing the drawing in the screen with zooming, position wrt the UCS icon, where the cursor cross hair is left hanging, suitable background screen color (white is a good choice), line color and thickness appropriate to the medium and the background color you changed to. (ie yellow on a black screen may be fine but yellow lines on a white background may be unacceptable.-aj)
1) You can leave the file as a drawing and insert it into word using: Insert...Object...Create from file...Browse...select your file
One tip: you'll want to save the mcad drawing in exactly the view you want to show in word.
2) Export to WMF format. Or even better, get BetterWMF from Furix (lets you control linewidth, color
etc.). We use this for all CAD-drawings inserted in Word documents
3) Print the drawing or desired view to a 'publish to web .jpg' file.You should be able to make this selection in you print dialog box. Then insert the image into your word document. We have found this method inserts
the best image quality. Be sure to set the hide lines option if the print is from model space.
4) Get the image you want on your screen. Print screen. Paste the image into MS Paint or a graphics program and save as whatever type of image you need. Insert Image into Word.
5) You might want to avoid raster and keep it in vector format if you can, or it will have the 'jaggies'. Also, jpg is a poor choice of graphics file, as it is 'lossy' compression scheme and will antialias away all your sharp lines. the easiest way is simply to get the view you want (make sure the backround is WHITE) on screen, select what you want, hit Edit->Copy, go to word and paste. you may have to fool with it a bit, but Word is actually very good at OLE and should handle it well. I spend half my life doing this at work, give it a try.
(..this is pretty good. just make sure you fill the sreen with the drawing and then you can re-size it down in Word and still see it ok. Beside making the background color (and hence the drawing colors) what you want, make sure the cursor cross hairs are out of the way. I pretty much oppose OLE from the point of view of linking because the dependencies you set up such as needing to have a particular version of Office and a particular version of the MCAD package that might not exist at some time in the future. But this is just copy-pasting not linking.
If you are happy with 4) but just want all black lines you can leave you original drawing alone and use export 2D views to a new layout. There you can change colors without altering you original drawing then copy/paste to Word. It takes seconds and works every time.
If you want a good line raster image of minimum file size for the web consider png, Word is happy with it and it will give you a minimum file size without the transitioning jaggies that occur in jpg at half the size of a gif for internet use.
This topic goes in and on. I use PaintShop Pro 7. It does everything I want without the cost or complexity of Photoshop but it would be unfair not to mention www.irfanview.com. and www.capturepad.com. which are shareware. MS Paint is fine but won't do png.
* Situation: Recently upgraded to MDT6 from MDT5, and I'm having a problem with regular old clipboard copy and paste. I got used to the quick and dirty method of pulling parts out of complex assemblies via copyclip and pasting them into a new drawing so that they could be saved as assemblies, which subsequently made them more manageable when re-inserted (via Attach) into an overall master assembly. Anyway, this worked great in MDT5, but in 6, any unconstrained parts are losing their general relationships to each other when pasted and are coming into the new drawing in all sorts of new and exciting orientations, which shoots my copy/paste extraction method in the head. Is there a setting or parameter that I'm missing that will allow me to maintain the orientation-as-copied of pasted parts?
Soln: Come in Assist>User preferences>click in Windows Standard acceleratorkeys Ok.
* Q: I'm using MDT6. We get a lot of customer iges files of 3D surfaced parts. When I igesin these files, a lot of the surface normals are facing the wrong way. When I shade the part for a quick look, you get a lot of 'holes' in the part. I then go through the part and flip the normals so the part will shade correctly. My question is there a way to quickly flip the normals so they all face to the outside of the model? I can't just window everything because half of the normals are already facing the correct direction.
A: If you just need to flip the normals for viewing only, go to Assist/Options/System/3d Graphics Properties and uncheck 'Discard back faces'.
If you need to adjust the normals for CNC, etc. go to Surfaces/Edit Surface/ Adjust Normals. You can window multiple surfaces and flip the normals for all of them.
* Q: I am trying to copy a sketch (actually just the lines that make up the
sketch) to another A'desk application. If you copy an entity or set of
entities in one file in MDT (edit-copy) you can then paste those entities
into another file. If I try to do this by editing a sketch and trying to
copy and paste the entities that make up that sketch to another session of
MD, nothing comes in - What am I missing?
BTW, ultimately this is an experiment where the sketch is to be used in
Inventor (7), so if there is an easier way to do this, please let me know.
* A1: I'm not sure if this applies to your case, but it is as designed in MDT that
annotated entities (like welding/surface symbols) and some others will not
come through when copy/paste is used. Make a local copy first, and then do a cut/paste, it should work then.
A2: Why not just open the mdt part in Inventor? Then if you want to rebuild there, most of the original sketches should be available to copy to new sketches in a new inventor part file. It's real easy to extract the sketches in inventor.
* In AMOPTIONS->Part, in addition to unticking Assume Rough Sketch when you dont want MDT to alter your sketch, you may want to consider unticking Apply Constraint Constraint Rules also (perhaps if you are getting 'zero length arc' messages also)
* Q: Can't measure in Z plane (get 0). Lines drawn lie on Z=0 (xy) plane.
A: There is a Ignore z check in the ampowersnap dialog. Unchecking it should fix it.
* Not sure what program made a dwg? Use Windows Explorer and RMB on the file. Choose Properties. If Custom tab look under Name column it has AmdtFileType and then a 84 or some other number close to that it most likely a MDT file.
* Q: I have a flat object that I need to drill a hole at 45 deg and at 30 deg. What is the easiest way to do this. the drill needs to start at a particular spot on the surface 1.250, 0.508 from 2 edges.
A1: Place a centerline on the surface to be drilled. Use the 'sketch' method. The centerline should be at the exact location of the hole. Place a work plane on the centerline perpendicular to the centerline of the hole, using the 'on edge/axis' method. Next draw a circle on the work plane and dimension from two edges. One of the dimensions should be trigged to compensate for the angle. The circle should be extruded 'midthru'. If you want to use the 'Hole' function of MDT, you should drill from an offset work plane or you will get a partial hole. Sincerely, Ralf.
A2: I use the same method as A1, but instead draw circle I place work point on the work plan and
dimensionally constrain it and than create hole using work point option.
A3: Here's how I usually do this...I create a small hole, and place a axis thru it, that I can use to rotate my work plane to the angle required...I do this in an area of my part that will be 'consumed' by a later operation (make the base part something much larger than needed), I then place a dimensioned work point to locate my hole...This method makes it easy for me to easly adjust the hole placement by moving the consumed hole around.
* (related to my problems reviewing other people's work on my machine elswhere on the network that made me look at eTransmit) If youve moved files to another computer and renamed all the folders etc to allow you to work on that project (or just look at it) and MDT still says it is looking for something in the drive of the other PC try RMB on the part you are concerned about, choose Show Definition and then check out the path shown in dialog box at the bottom. It should show the current path, if not, use the browse button to set it properly - make sure you hit 'save path' before leaving the dialog box
.Q: I have created a broken view of a 3D solid using AMDWGVIEW, however the view does not have the customary break lines seperating the broken halves. How do I turn them on or create these lines?
A: You have to add them manually using AmZIGZAGLINE (not in MD4 -aj) and then annotate them to the view (amannote-create) to make them stick to the view if it is moved or changed. We do this a lot and it is a bit of a time consumer.
* Feature Exchange
Q: I need to work with an imported SolidWorks step file. It seems that the resulting solid cannot be edited but it can have features added to it. Is there some way to retrieve the parametric data so that the original solid can be edited? Or must I recreate the solid instead?
A: Step does not carry any parametric data with it. That said you should have a 30 day trial of Feature Exchange on your install CD that will try to rebuild the part with features. (From Cadalyst MDT6 intro article "An extra-cost Feature Exchange add-on module transforms solids into fully parametric parts. The STEP translator is now built in, and you can batch convert multiple solids in a single step".
* AutoCad 3D model into MDT using ACIS (.sat) (OR MDT model into Vanilla AutoCad)
I was sent an MDT 6.0 3D file from a vendor. I have AutoCAD 2000i. We need to get dimensions off the model but the object is a Proxy Object. I need very accurate dimensions from this MDT model. Is there any way to get them without buying MDT (using straight AutoCAD)?
A1: Other than they should have sent you fully dimensioned layouts (2D drawings) they they could export an acis (.sat) file that you could import directly into Acad.
(In MDT use File->Export->ExportData->(Export Data dialog box) Save As Type: ACIS(*.sat).
Note the other 7 options: wmf, stl, eps, dxx, bmp, 3ds and (block)dwg.
Note the other two Export options where DesktopVRML and IGES (STEP was greyed out) -aj)
More simply stated use You may use the command AMACISOUT instead, and then ACISIN into ACAD.
A2: Is this in a part drawing as opposed to an assembly drawing? If so, open a new 'assembly' drawing and attach the part. Localize the part, make it active and you should be able to explode it. From there you can cut and paste it into Acad 2002 to get rid of proxies
* What is AMMODELINFO? It occurs in a lisp from www.mymcad.com mdtfaq5012 in Nifty Routines. Asserted to run on MDT4 and command line does accept it but does not occur in MDT4 Help's Command or System Variable listings. Only Google reference is the same mdtfaq5012. The lisp sets it to 'L'.
Q: Does anyone know of a macro or lisp file that will tell you what all higher assemblies a part is used in. The assembly has gotten to large to track from the top down through the subassemblies and I need a way to track how revision changes will affect assemblies higher on the tree.
A: Gary McMaster wrote a VBA program that will put a assembly tree into Excel. You could
track it in the excel file fairly easily I would think. You can find the Assembly Tree program on my web site
www.mymcad.com/KWiK/mdt/mdt.htm
Q: I get a lot of customer files in IGES. Maybe half the time, they only give me one side of material shown on a sheet metal part. Anyway, after I've offset all the surfaces to the proper metal thickness and then applied surfaces to the edges of the model, when I try to stitch it to a solid, it fails and becomes a quilt. When it fails, is there a way to locate the offending surface(s) that is causing it to fail? When I shade the part, visually it looks watertight.
A:Can you use amthicken instead? This will turn the surface into a solid directly instead of offsetting the surface and creating all those edges. Try it two ways. If the surface is actually several sufaces stitch them together first then amthicken. This doesn't always work. Alternatively amthicken each piece and then amcombine. Another alternative is to create a solid block and then use amsurfcut to cut away unwanted portion.
(aj -see also acadmdt/quilts/quilts.html MDT Quilts.)
* Constrain a washer on the top center of a slot (MDT4,5,6,7).
Note. When constraining two parts, the part lower in the browser tree will relocate itself on the part which is higher in the browser tree. This can be disconcerting when you are constraining a minor part to a major part and the major part relocates itself onto your casually placed minor part. If this is a concern you may wish to drag a part which is lower in the tree up above another part. With MDT4 it's just left click and drag but for MDT5,6 and 7(2004!) you have to also hold down Shift.
First constraint (face to face):-
Right click->(Assembly Menu...)->Constrain 3D->Mate the bottom face of the washer to the top face of the slotted body. You may want to MOVE the washer to one side before commencing the next mate.
Second constraint (center of slot lines to axis of washer ..the tricky bit):-
Step1. Right click->Constrain 3D->Mate again and select one of the top slot lines that the washer will eventually sit on, left click again (once should do it) until the center of this line is highlighted (do not right click to accept this center point!). Now hover the cursor over the other top slot line (the mouse cursor tip will turn back into a selection pickbox) and left click to select it. Left click again until that lines center point is also highlighted. Still do not right click to accept anything! Now tap m (for Middle) at the command line and the middle of the slot will be indicated. Ok NOW you can right click to accept.
Step2. Left click on one of the circles of the washer which highlights the washer axis, right click to accept that axis and right click again accept the zero offset.
Done!
* OSMODE MDT5
(An Autocad system variable. Sets running object snap modes using bitcodes.
eg OSMODE=55 (one posters favourite) is a certain selection of OSNAPs? My MDT4 was 311.
* Succinct statement about Inventor.
If they have a lot of legacy 2D Acad files I think they will be much happier
with Desktop.
If you have inventor you will need to have a way for others to work with the
files - if they are used to working in model space/paper space MDT will be
very natural for the other drafters that have to maintain the files.
Inventor's Acad compatibility is no better than the other mid-range modelers
and in some ways it's worse.
If you go to inventor you need to manage multiple files for each part and
you need to have everyone on the latest and greatest hardware. Most AutoCad
shops don't have the file management system needed to deal with Inventor -
if you are a one man shop that works only on a project basis you can do it
with Design Assistant. If you have multiple people that need to work with
the files and are trying to coordinate with legacy data it could be a bumpy
ride.
If he is trying to open their eyes to the advantages of 3D while most people
still work in AutoCAD - MDT would be the way to go. If you think you can
get management to do a real switch I would investigate all the
alternatives - not just Autodesk.
* Just want to raise a concern here,
Q1: Why is it not possible to save a file in MDT2004 (saveas...) to MDT6?
A1 Saving a file back into a previous version has never been and never will be
possible in any 3D modeler (Leo Laimer)
Q2: But Inventor 7 files are backward compatible with Inventor 6!
A2: IV7 in reality is IV6SP3 and yes, it uses the same file format (Leo Laimer).
* Sun Angle Calculation (MDT4,5,6,7)
Type LIGHT on the Command line. In the Lights dialog box, select Distant Light (uniform lighting that simulates sunlight) from the dropdown list and select the New button to the left of the dropdown list. This brings up a new dialog box, where you can set up the properties of the light, which also includes a Sun Angle Calculator.
* What I do when I want to know the number of solids in an assembly: AMACISOUT, open new file, ACISIN, delete/all.... commandline says '..xyz entities selected...' Works great even for very huge assemblies (Leo Laimer).
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