Printable View
Hi could someone please tell me the correct settings in solidworks for this linear profile rail. its telling me on the diagram that the bolt size is 4.5mm but when using hole wizard im struggling to find the right settings for a tapped hole. or if i just use standard holes and setting dimensions im only seeing radius so do i just half that so if my hole is 4.5mm i enter 2.25mm in the radius dialog?
cheers
Ash
The rails have larger than normal clearance holes to allow them to be adjusted as needed. If your rails have 4.5mm holes and they are screwed in from the top, you will need to make M4 tapped holes. The pilot hole for a tapped M4 using a cutting tap, as opposed to a rolling one, is 3.3mm.Quote:
Originally Posted by reefy86
The pilot holes are always=nominal diameter-1 pitch length. So an M6 will have a 5mm pilot, a M5 uses a 4.2mm pilot etc.
thank you very much :)
so just to double check. if i make holes in my drawing thats 4.5mm and send that drawing of to be drilled will they tap my holes at 4.5mm or will they just do a basic straight hole at 4.5mm?
cheers
Ash
im not using the hole wizzard btw im just using a standard 4.5mm circle with an extruded cut.
cheers
Ash
depends if you send them a drawing or a solid model. As a rule, you should not send a solid model without a drawing to ensure your intentions are met. For example, a solid model may not convey tolernaces.
A 4.5mm hole is just that. Unless you tell them to tap it to an M4, you will not get at tapped hole. Also worth noting that if you can accept a drilled hole, make a note that the drill point is acceptable. Flat bottomed holes are marginally more expensive.
thing is though that really confuses me is when looking at the dimensions from zapp it just shows a diagram with an hole at 4.5mm, im not good at knowing what holes what but in solidwork i select m4 and it has a default settings at 10.10mm blind hole depth and 8.00mm tap thread depth.
Slightly confused myself here too. What are you trying to draw up, the rail or the mating part?
If it is the mating part:
That setting is fine if you want a threaded hole. It give you two full diameters worth of M4 thread. I am sure you know you cannot tap to the bottom of a blind hole so the 10.10 is pretty decent in my mind.
As have been said A 2D drawing is best and if you are asking for holes to bolt the rails to, through holes are much easier to drill and tap. As long as the hole centres are marked and dimensioned on the drawing that will be fine. You can just say drill for M4 or M5 or whatever size you want, the company would then drill the appropriate hole.Quote:
Originally Posted by reefy86
forgive me for sounding dumb, so if i ask them to make an m4 hole will they know to tap it or will i have to tell them.
its for the linear profile rails.
Never assume that the machine shop knows what you mean or need. You can however be as descriptive as you want. For example, you add an arrow to the threaded whole with a note leading from it saying: 24 X M4x0.7 8mm MIN FULL THREAD. DRILL POINT OPTIONAL TO DEPTH 12MM
thank you :)
When i send to somebody some things to machine for me i do the following:
/thats how i like to receive also/
- on the 3 D drawing i group all same plate thickness objects at one plane and near each other and send each group as separate file.
The file is accompanied by another JPG snip which shows basic dimensiones, so when you take a glance you could see more or less what the job dimensions are.
-Each piece has detailed snip or even some times 5, with hole detailed explication, where tapped, where pass through, hole clearance, etc.
What i hate to receive is 15 separate files and i waste 2 hours to import them and check dimensions only to give a quote. When they are grouped i could import them at once and could judge material weight, hence price for a minute, not another hour.
if machining 5 parts that go together, i want also to see how they interact, so i always need also the assembly file with them. 99% of the files i have seen or have a design mistake, something not well thought or is done from people who dont have any idea how this will be mounted together in real life.
I have yet to see something that does not need any correction. dealing with fellow DIY crowd i mean.
thank you that makes alot of sence to do it that way tbh and feels natural.
cheers
Ash
just to throw something in there would this make sense for you guys or does it look confusing :)
Attachment 17622
I think you have too many measurements some are duplicated also the bottom 4 holes are drawn differently ie not showing the countersunk bit. I don't see the line down the centre holes sizes. If all the holes are the same size you can say that. Unless the holes tapped just say the hole size ie not M8 8.1 as a M8 hole would be 6.8mm to be tapped.Quote:
Originally Posted by reefy86
If hole are through holes I would say that instead of 30mm.
I would reference all the measurements from one end and one side. Do you really need 30mm plate?
Do you have a dxf file for this. If not I can do one for you.
Just to add to what Clive says, I don't see any measurement for the actual position of the 4 and 8 grouped holes on the plate, try and pick two sides(Datums) to take the measurements from and maybe positional tolerances if its important to you. Also you don't need the length of the angled side, an angle would do.
Cheers, Charlie
ahh yeah sorry i forgot about the position of the holes, as for the bottom 4 the reason why they are different is because the counterbore are on the opposite side. i do not have a dxf file as im new when it comes to drawing so that was actually my first drawing to show you guys lol.
cheers
Ash
forgot to mention i want a close fit on the through holes so instead of 8.4mm i wanted 8.1mm thats what i meant to of said.
Ash
If you want alignment, use dowel pins or shoulder screws not plain screws. tightening the through holes will cause tolerance stackup issues.Quote:
Originally Posted by reefy86
Well then you have not said on the drawing which side is being countersunk. You have not mentioned 8.4mm only 8.1mm. If you say you want a hole for M8 it will probably end up at 6.8MMQuote:
Originally Posted by reefy86
So
1: Do you need 30mm ali
2: You don't need to say M8 just the hole size you want and whether it is through hole or to a depth
3: set all your measurements from two datum's ie bottom and one side.
thanks guys, 30mm probably is ott what would you recommend for all round? i think i will stay with 30mm on the front z axis plate though but for everything else would 25 do? i know 20 is the minimum.
and with the holes so i just say 8.4mm through on plate 1 and 6.8mm tapped 15mm depth on plate 2?
Ash
How big is this machine I would have thought 20mm would have been enough for gantry ends and Z axis.Quote:
Originally Posted by reefy86
You said you wanted 8.1mm so now you are saying 8.4 !!!.
You have not mentioned plate number 2 If you want them to tap the holes just say tapped for M8 x 1.25 if that is what you want. You can't just say 6.8mm tapped
I would suggest you re do the posted drawing with the measurements as shown etc
above post mentioned tolerance stackup issue with tighter holes which is why i went back to 8.4mm. plate 2 was me trying to say i want a m8 cap screw to go through plate 1 and then screwed into plate 2 which is tapped ect. i apologise for my bad explinations. and machine cutting area is 8 x 4.
cheers
Ash
Have you put a drawing up about the machine gantry etc? Dean might be best to comment on plate thickness.Quote:
Originally Posted by reefy86
Bullet points are the best on separate lines to stop confusion when asking a question (just be blunt)
just a quick one. if im using shoulder screws do i do the through holes 10mm which is what the shoulder screw is or do i make it slightly bigger like 10.1mm. dont want to make a mistake of inserting 10mm shoulder into 10mm hole and it gets stuck ect
Ok, shoulder bolts are ground to specific tolerances on the shank. Depending where you get them from, there will be a tolerance class to them like h8 or something. That will tell you what hole size and tolerance you should specify depending on the tightness of the fit you want. Give us a link to the bolts.
This is where geometric tolerance will also come in to play but that may be overkill for your application.
Are you looking to get this made by a chap in a shed or are a pro machine shop?
just in general i was checking ebay out for the shoulder screws
http://www.ebay.co.uk/itm/10mm-M8-SO...DKYqt_xV0EeV8A
states nothing about tolerance just simple dimensions ect. although here it has more technical info but £3.44 per screw jesus lol.
http://www.shoulder-screws.co.uk/?gc...LnEaAskt8P8HAQ
Shoulder screws are ground to specs, so a 12mm shaft shoulder screw is 12.00mm, see picture below. So i just drill a 12mm hole with a good new Dormer drill bit.Quote:
Originally Posted by reefy86
Attachment 17633
thank you. just dont want to be making any mistakes in my drawings and want everything to bolt together nicely the first time.
Ash
ok, the precisionist in me is screaming right now because I work with drawings, precision and accuracy on a day to day basis.
Everything has a tolerance, even ground shoulder bolts. A vernier caliper is not the golden standard as it has a 0.02+/- accuracy tolerance. A micrometer on the other hand is the standard. Would you need this kind of precision for your application? That is your decision.
Now when you use a 12mm drill, you are likely to get a 12.1-12.2mm hole. If you want an accurate hole, you need to ream it.
This is getting silly now just use standard cap head bolts like everybody else doseQuote:
Originally Posted by reefy86
i dont mean to make this thread all pointless and silly, i have no real experience when it comes to cnc or mathmaticals unless its your typical diy timber frame that any dummy can do. now the cap head bolts was what i was using but then the shoulder screws came into it :). now ive read hundreds of threads and love them all and watched plenty of videos to know that there cant be any play in the machine regardless if its just cutting wood or aluminium so this is the reason why i asked about clearance hole size because when looking at the drill tap and clearance chart it tells me the clearance for an m8 bolt is 8.4mm but the bolt is 8mm so i asked if 8.1mm clearance hole would work and then i got told id get tolerance issues. everyone who is helping me here has their reasons and know what they are doing and i apologise for confusing people :)Quote:
Originally Posted by Clive S
Ash
Another way to look at this is that if you have access to high-precision machining and manufacturing facilities, you can make parts to incredible accuracy and just assemble. That's how car manufacturers work these days. If you are building with typical home workshop facilities, build with a bit of slack at key points and then align on assembly. That would never work commercially but with care and a bit of extra time, it can give good results. So I would go for 8.4mm clearance holes, for example, to give a bit more wiggle room on assembly. If you want to lock parts after setup, you could drill and ream through both components and fit dowel pins but I doubt if many do.
You having a laugh.!! Drills are about much good at making accurate holes as I am at pole dancing.!! The whole point of Shoulder bolts is precision and this requires reamed holes.Quote:
Originally Posted by Boyan Silyavski
I've not commented here because Ash has been in touch via email so I've told him this already but I'll repeat again here for the sake of others reading this who are just thinking about building.!
At DIY level building in lots of adjustment at the start is priceless when the machine built and your setting up chasing accuracy etc.
With all the best will in the world and careful marking etc there is point that without High precision machinery to help with build then your always going to need adjustment or wiggle room.
This doesn't mean high accuracy can't be achieved at DIY level it just takes lots of time and patience.
Ash,
Keeping it simple - to bolt part A to part B with a flush fitting M8 cap head:
1. If you are doing the work:
Part A- scribe centre of hole, use centre punch, spot drill and then drill a through hole with diameter 8.5mm drill
Part A- use an M8 counterbore tool (has diameter 15mm) to a depth of 8mm (same as M8 cap head depth)
Part B- mark out, centre punch, spot drill, and then drill a pilot hole of 6.8mm diameter
Part B- use an M8 x 1.25mm tap to create the thread (keep it straight in the hole)
Tidy any raised burrs left on either side of part A or B using a countersink tool - otherwise they will not sit tight against each other
__________________________________________________ _____
2. If you are making a drawing for someone else to make:
Part A- label hole circle as "dia 8.5", label counterbore circle as "CB dia 15x8"
Part B- label hole circle as "M8 x 1.25" (they will know to drill it 6.8mm, tap it, and do the countersink tidy up)
If you have multiple holes which are clearly all the same you can use " (xx places)" after the dimension. For example if you have 5 holes all the same you can label just one with the text "dia 8.5 (5 places)".
__________________________________________________ _____
Notes:
Be aware that an M8 bolt is actually slightly less than 8mm in diameter so the hole could be 8mm but the 8.5mm clearance will give you some adjustment. I use 8.5mm (rather than 8.4mm) because 0.5mm steps come in the regular drill sets, although you can buy drills in various sizes such as 0.1mm steps.
If for some reason when you put it all together that you need a bit more adjustment to account for slight errors in other parts, it is no big deal to drill the 8.5mm hole out to 9.0mm, so don't sweat the 8.1 vs 8.4 vs 8.5 dilemma. Important thing is to get a hole in the right place.
If you have a more complex part with counterbores on the upper and lower surfaces (or any detail on other faces) then you need to draw all relevant views. To understand this read up about 3rd angle projection which is a standard for laying out the top, side, bottom, front, back, of any part in an unambiguous way that the machinist will understand.
If you try to label a counterbore on the underside of the part by pointing to it on the upper surface drawing you will cause confusion and might get the CB on the top instead.
Spot on:yahoo:That's exactly what I was trying to say very well put.
thank you very much for that, as i mentioned to dean i was trying to make everything as zero tolerance as possible which for a diy machine its pretty much impossible to do that and was reading way too much into things so sorry for all the confusions :)
Ash